Linear Buckling Solution 2

[jetmaker]

Does anyone know if the linear buckling solution (SOL105) in NASTRAN accounts for bending due to load eccentricity?

Problem I have is a C-channel loaded on the flanges such that it causes a bending load as well as axial compression in the web. Trying to determine if the eigenvalue accounts for this or not.

Thanks.

jetmaker

 

[271828]

From your description, it seems that your problem probably has a nontrivial solution. In other words, you apply some little bit of load and get some movement. In other words again, no bifurcation is possible.

Unless I'm mistaken, an eigenvalue buckling analysis won't work in this case.

I could be wrong, though. I'd run a series of simpler models, working my way up to the real one until I understood exactly what the program was doing.

 

[271828]

I played around with SAP's buckling feature and convinced myself that it doesn't handle cases like yours correctly. Your program also might not.

Then again, it's late on a Friday night, LOL, and I've been known to be wrong before.

I tried this problem: Pinned-pinned column, internally subdivided. Concentric load = 1 kip. Use eigenvalue analysis to get the multiplier. Multiply this by 1 kip and it matched the Euler buckling load perfectly.

Then I changed the problem to have a concentric load = 1 kip and a small moment. Remember the multiplier should be multiplying ALL loads. Run the buckling analysis and the answer is the same.

Then I changed the problem to have a concentric load = 1 kip and a very large moment--exact same result, obviously bogus. With the moment I put on there, a tiny P should cause huuuuuge displacements.

These buckling analyses work by solving the eigenvalue problem using the elastic stiffness matrix and the geometric stiffness matrix:

[Ke + lambda Kg]{phi}={0}

Solve for your load multiplier, lambda. For framed structures, Kg is filled with a bunch of constants * P/L. Shells should be similar, although more complicated.

Depending on your problem, the algorithm might do the same thing. If your eccentric load doesn't cause Kg's P's to be different, then the algorithm will not take them into account. I guess it depends on the problem--some eccentricities might change the P's.

 

[pbd999]

Nastran Sol 105 will give you the linear buckling load, but when you have a beam column (eccentrically loaded column) the real failure load will always be less than the linear buckling load. The linear buckling equation includes the stress stiffness matrix (MSC calls it the differential stiffness matrix) which only includes the state of membrane stress. If you look at this matrix it doesn't have any reference to moments or inertias or anything related to bending. Tensile stress makes the structure stiffer, compressive stress makes it softer. You can make the eccentricity or initial moment as large as you like and it doesn't change the buckling load.

If you look at a textbook for eccentrically loaded columns, you see a load-deflection curve with the buckling load shown as a straight line across the graph at some level. This is the linear or eigenvalue (i.e. perfect, Sol 105) column load. If there is an imperfection in the column it immediately starts to bend as it is compressed, with this bending causing more eccentricity, which causes more bending, etc. This effect can only be captured with a nonlinear finite element analysis (Nastran Sol 106). Back to the textbook plot, curves of increasing eccentricity or moment approach the "true" buckling allowable asymtotically, but they will likely fail by bending stress before they buckle. I call this the plastic collapse load, rather than the buckling load. In Niu's "pink" Stress Analysis book Fig. 10.1.1 more or less shows this.

 

[jetmaker]

pbd999,

Ok, so you and 271828 have confirmed my suspicion: that SOL105 only solves for the EULER buckling load and does not account for any non-linear effects.

You seem very knowledgeable with NASTRAN and I need to run the non-linear buckling solution to obtain the proper results. Could you help me with this? I am trying to find the steps involved and would be interested in some documentation/tutorial on how to do this. I am following an example right now from NASTRAN, but I can not seem to get it to work for my application.

Your help is greatly appreciated.

jetmaker

 

[pbd999]

I can give only the basics...it can get complicated and is so problem dependant. Instead of Sol 101, call out Sol 106. In the Subcase section you need to call out the NLPARM from the bulk data section. Use PARAM, LGDISP,1 to turn on large displacements. You have to have an NLPARM card in the deck. Like so,

$ Nonlinear Static Analysis
SOL 106
$ Direct Text Input for Executive Control
CEND
TITLE = MSC.Nastran job created on 09-Nov-06 at 11:49:55
ECHO = NONE
$ Direct Text Input for Global Case Control Data
SUBCASE 1
$ Subcase name : Default
SUBTITLE=Default
NLPARM = 1
SPC = 2
LOAD = 2
DISPLACEMENT(SORT1,REAL)=ALL
SPCFORCES(SORT1,REAL)=ALL
STRESS(SORT1,REAL,VONMISES,BILIN)=ALL
$ Direct Text Input for this Subcase
BEGIN BULK
PARAM POST 0
PARAM AUTOSPC NO
PARAM LGDISP 1
NLPARM 1 10 AUTO 5 25 NO
$ Direct Text Input for Bulk Data
$ Elements and Element Properties for region : panel
PSHELL 1 1 .04 1 1
$ Pset: "panel" will be imported as: "pshell.1"
CQUAD4 1 1 3 49 48 1
etc...

For the first run through use the defaults for NLPARM and let 'er rip. It will divide the load into 10 increments initially. See what happens. Since you are dealing with buckling at some point the solution will not converge anymore but that is not really a disaster...it just means you may be close to the physical instability point. It sounds so simple but it's not. NL FEA can be an order of magnitude more difficult than linear to figure out if your answer is "right". You should talk to someone you work with that has done it before...