Inelastic column buckling 2

[dozer]

I've been playing with COSMOS/M using it to analyze a simple truss with a uniform gravity load on the bottom chord. Simple hand calcs indicate that the center of the top chord will be the critical element and it will buckle in the inelastic range. I ran a linear buckling analysis and got an eigenvalue that agreed very close with what I would have got if I checked the chord as though it were in the elastic range.

I want to understand what "really" happens but not being very familiar with nonlinear buckling analysis, I farmed it out. This analysis (using ABAQUS, spelled?)indicated a load factor at failure (ie; muliplier on load that caused buckling) slight higher than the eigen solution. What puzzles me is I would have expected a slightly lower value because I thought it was going to be in the inelastic range and the chord failed at its yield strength which suggest to me it didn't fail by buckling at all. (Yes, material nonlinearity was included.)

Here's my question, can a nonlinear analysis accurately predict inelastic buckling? If so, what is the secret to getting it to do so?

At the risk of boring you let me add to my description. One of the things I'm really trying to get my brain around is reasonable k-values for truss members. Text I've read recommend a value of one for chords, the theory being that if a member adjacent to another member wants to buckle at the same time it will offer no rotational stiffness at the joint. When I ran the linear buckling this is exactly what the deflected shape indicated. The top chord to the left of center buckled one way, the adjacent chord to the right of the joint buckled the other. Thus the joint that was common to both of these members rotated. This makes perfect sense to me but the nonlinear analysis I had run is not showing this. My fear is my managers will look at this nonlinear analysis and say "See, you can use a k much lower than one." But physically I just don't believe it. My suspicion is one or both of the following:

1) The program is not doing inelastic buckling correctly. (Hence my original question.)

2) The program is not accounting for the loss of stiffness when two adjacent members are loaded at the same level.

Thanks in advance,

Randy

 

[pd]

rkillian

A couple of observations on your question.

Firstly, in order to get "decent", believeable results out of a 2nd order buckling analysis, I have found that you usually need to apply either a small lateral load (say 1.5 % of applied axial compression force) or a small lateral out-of-straightness (say L/500) to "disturb" the system. Otherwise, you appear to get large capacities out of sections which you know would otherwise tend to buckle. You can compare results with BS 5950 blue book to start to get a feel for whether you are in the right ballpark.

Secondly, BS5950 k-values always seem like alot of hardwork. It appears quicker to use some form of computer analysis.

Thirdly, assuming that you do use these to help give you a hand-calc feel, then the adjacent elements will always provide some degree of rotational or lateral stiffness to the element under consideration. I may have misunderstood your email but it appeared that you thought that the adjacent element provided no stiffness to the element under consideration.

Hope the above helps a bit.

Cheers
pd

 

[dozer]

pd,

Regarding your third point. What I meant was that if a member framing into the member being investigated wants to buckle at the same load as the member being investigated, then you cannot count on this member to provide rotational restraint at the joint.

Hmm, that was a lot of "members" hope you followed that.

rkillian

 

[brad]

There's a lot of factors at play here which may have caused the result you saw.
The simple answer is that this is certainly possible, and not at all unlikely, given certain sets of assumptions..

Depending on your material curves, there may have been material hardening at play.
In the actual analysis, were truss elements used? If instead beam elements (or other types) were used, then there certainly could've been a higher critical load than would've been predicted linearly.

I would not initially expect the behavior which you described if truss elements (meaning axial-bearing only) were used, and if an elastic-purely plastic material was used (meaning that there is no more load-bearing capability after initial yield). Any other combination could conceivablyresult in what you saw.

I agree with pd's statement about axial loads and/or out-of-straightness. As you stated that ABAQUS was used for this, make sure that *imperfection was used in this analysis. In ABAQUS that is used to give an initial imperfection which results in more conservative answers. If that is not used, then the structure may be numerically "perfect", resulting in unrealistically high loads. I would be very concerned if that were not taken into account in this analysis.

One last thing--technically as soon as you're doing nonlinear analysis, it is no longer "buckling", but rather critical loading. It may be that your critical load is indeed higher than a buckling analysis would calculate; however I would be wary in changing my factors of safety by much.

Brad

 

[dozer]

Thanks for the replys guys. Since, I originally wrote my question I've "buckled down" (pun intended) and done my own nonlinear analysis. As I mentioned, I wasn't entirely pleased with the results I got back from the guy I farmed it out to. I don't have ABAQUS, rather I have COSMOS/M. I took pd's advice and after running it with straight members, I put an out-of-straightness in the two critical members of L/500. If COSMOS/M has an *imperfection option like Brad mentioned that ABAQUS has, I'm not aware of it. Anyway, it went from a load factor at critical in the "perfect" condition of around 3.0 to a load factor at critical of the "imperfect" one of about 2.2. Quite a difference.

BTW, Brad, to answer your question. I'm afraid I used the term "truss" rather loosely. The elements are 3D beam elements and the joints are moment carrying. The structure looks like a truss but it is not one in the strictest sense of having pin ended members and being loaded only at the joints. I'm reminded again of how important clear communication is . . . and probably still falling short.

Again, thanks for the help. As I'm new to nonlinear I'm going to have more questions, but I'll save them for another thread and another time.

rkillian

 

[chandr]

rkillian

From the point of view of a stuctural designer, I'm not sure what's the purpose of your inelastic critical load analysis. If the purpose is to get a realistic failure load, I wonder if it does have any useful values if the residual stresses are not realistically put into your members. Then you'll still get the failure load higher than the one from experiments or code curves. If it's for evaluating the forces in the 2ndary members such as bracings, this's worth but I don't think you need the mat.nonlinearity. The normal practice of truss design I did and saw is to perform elastic bckl and use code formula to get the allow.load, then do nonlin.elastic anal. to get the forces in bracings.