×
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS

Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here

Jobs

column buckling check
2

column buckling check

column buckling check

(OP)
I tried following the procedure in this thread (suggested by 271828) to get a column buckling load out of a program, but it just isn't working.  It keeps upping the lateral displacement, but it never becomes unstable near (or above) the elastic critical buckling load.  I could double the euller buckling load, but the lateral displacement is always appropriately proportional.


thread507-211026: Column Effective Length

RE: column buckling check

What program are you using?

What type of analysis?  Small-displacement P-Delta?
 

RE: column buckling check

(OP)
RAM Advanse.  I broke a 20' column into 2' segments and modeled a half sine wave.

RE: column buckling check

Does RAM Advance do a PΔ analysis?

 

RE: column buckling check

I mean technically...a second order analysis since you have intermittent joints along the length.

 

RE: column buckling check

(OP)
Advanse does do a P-big delta analysis.  It doesn't do the P-little delta analysis (hence the broken member).

RE: column buckling check

Are you modeling it as a frame element broken into 2' segements??  

RE: column buckling check

"I could double the euller buckling load, but the lateral displacement is always appropriately proportional."

THis makes me think you are running a first-order analysis.  Are you sure the second-order feature is turned on?

Also, you might try the AISC App. 7 Commentary benchmark problems to make sure RAM's second-order analysis actually works.

RE: column buckling check

For all those who have already tried to compute p-δ moments using computer programs, here is a question:

Do you only have to divide a frame element into finite pieces to capture p-δ or should you break them into finite pieces and also introduce a "kink" in that node?

RE: column buckling check

It depends on exactly what you want to do.  Usually, you only have to break up the member.  After some load is applied, the nodes are displaced transversely, so the second order moments can be generated.  This would also work for eigenvalue buckling analysis.  Actually, I don't think eigenvalue buckling analysis would work correctly in most cases if the nodes were displaced initially--there would be no trivial solution, hence no eigenvalue problem.  Not sure that this is always the case, though.

In StrlEIT's analysis, he is trying to compute the buckling load for a specific mode using a very specific kind of analysis.  He needs to displace the modes into the shape of the mode that he's looking for.  If it's simply supported on both ends, then this initial shape is something like a half-sine wave.

RE: column buckling check

Don't you have to use brick elements to perform an eigenvalue buckling analysis??   

RE: column buckling check

No.  All you're doing is solving the following equation:

([Ke] + Lambda*[Kg]){Delta}={0} where

[Ke] = elastic stiffness matrix (the one everyone thinks of as the "stiffness matrix"

[Kg] = geometric stiffness matrix

Lambda are constants.

Of course, {Delta}={0} is a solution, but that's worthless to know.

If you set the determinant of [Ke]+Lambda*[Kg]=0, you get values of Lambda that correspond to non-trivial solution--hence the term "eigenvalue analysis."  These relate to the buckling loads.  Corresponding {Delta} are the modes.

[Ke] and [Kg] can be for any kind of element.  [Kg] has P's in it if you have frame elements, membrane stresses if you have shells, etc.

RE: column buckling check

(OP)
I modeled a 20' column (broken into 2' segments) with the half-sine wave, deformed shape of 0.01sin(pix/L).  This gives an initial displacement of 0.01" at mid-height of the column.

I'm working with W8x31 (arbitrarily decided on by me).  I have the buckled shape modeled for weak axis buckling.  I'm coming up with a critical elasic buckling load of right around 185K (on paper).  The problem is that the program is giving me results that aren't making sense to me.  The lateral displacement that increases upon initial loading (as expected).  What isn't expected is this - The lateral displacement stays small up until around 100k (it's around 0.17"), from there it starts jumping up faster.  At 135k, the lateral displacement is 0.28", at 170k it's 0.82", at 180k (just below critical buckling) it's 1.4" (like it's already buckled, but I would have expected much higher displacements for a buckled shape), at 190k (just above critical buckling) it's 3.8" (again, possibly buckled, but I would have expected much higher displacements for the buckled shape).

Here's the real kicker.  At 200k, it's buckling mode changes.  It jumps from the buckled mode that I assumed to a half-sine wave in the opposite direction (i.e. my assigned half-sine wave had positive 'displacements', but the buckled shape half-sine wave has negative displacements) and of much larger magnitudes (6.9" at mid-height), more along the lines of what I would expect from a critical buckling load.

Any ideas?

RE: column buckling check

Post the file.

RE: column buckling check

I did the same thing in SAP2000 except with a 1" initial center displacement - buckles around 185ish.  

Loads and center displacements as follows:
160k  -6.6"
170k  -12.19"
175k  -19.64"
180k  -46.58"
185k  -156"

RE: column buckling check

(OP)
was there a reason you chose 1"?  I tried to keep the initial displacements very small (thinking that the buckling behavior would be more pronounced).

RE: column buckling check

Check the basics of your model.  I just repeated your problem and my first one screwed up because of a basic boundary condition problem.

Here's what I did.  Maybe there's something in there that'll help:

Create 20' long beam of two frame elements with a node in the middle.  End nodes are set up to create a pinned-pinned condition.  Move the middle node 0.01" and auto submesh the members to get nodes at 1' apart.  Note that the initial shape is not exactly a sine wave.  This won't matter in the end.  It's close enough to the mode shape we're after.

Give the W8x31 zero shear areas to ignore shear deformations (your issue might be this or something similar).  Give it 1000x bigger area so axial deformations won't make the plot hard to read in its deformed shape.  

Use P-Delta, which solves [Ke+Kg]{Delta}={F}, so no iteration is required.  No need to use P-Delta plus large displacements option that would move nodes and iterate.

Pe = 184.352 kip

Results:

P (kip)   Delta (in.)
170       0.0961
182       0.6272
184       4.229
184.32    45.68
184.349   403.0
185       -2.32

The shapes look like half sine waves, but I didn't pull numbers out and verify mathematically.

Try to see what happens between 190 kips and 200 kips.  My guess is that your model has something in it that causes a little more stiffness than that used to compute Pe, and you'll see the deflection take off somewhere between 190 and 200 kips.

RE: column buckling check

"was there a reason you chose 1"?"

Either way should work.  Like you typed, the displacement will more suddenly increase with smaller initial displacement.

RE: column buckling check

Oh yeah, I used SAP2000 also.  I have no way to read a RAM Advanse file.

RE: column buckling check

It doesn't look like the program knows in the analysis that the column is unbraced (whether x or y direction) and buckles, the steel design check is run separately from the analysis. It is just keeps going through the displacements without considering a buckling point.  

RE: column buckling check

(OP)
haynewp-

I actually thought that until it buckled in a different mode than I originally assigned (which is making no sense to me whatsoever).

RE: column buckling check

I see where you said that above now. It looks about 196 kips it buckles and at 197 kips it is going the opposite direction. At 196.5 kips I get 124" of displacement.

I tried modeling it without the initial curvature and it never buckles.  

RE: column buckling check

Try 196.29 kips, I get 2754 inches in the positive direction then it switches at 196.3 kips to negative deflection.

I don't know why it never represents buckling if you take out the initial curvature.

RE: column buckling check

If you run your model without the second order option checked, it doesn't buckle. I think what we are seeing is the p-delta blowing out without considering column buckling.

RE: column buckling check

I used the same 20' model, with W8x31 weak axis bending on RISA 2D.   Had to put in an initial offset of 0.06" before it would register any second order buckling (might be a round off of cooordinates within the solver).

Here's my results:

Load           Defl at midpoint
           w/o Shear Def.    w/ Shear Def.
100 k         .058"             .058"
150 k         .207"             .210"
175 k         .808"             .842"
180 k        1.561"            1.695"
185 k        13.86"           42.30"
186 k       buckles            buckles

Per AISC 13th Edition - Equation E3-4, Fe x Ag = 184.9 kips

 

RE: column buckling check

I forgot to mention for the above numbers - I also divided up the member into 1 ft. segments with PΔ turned on.   

RE: column buckling check

JAE, what buckling value does Risa give if you run the same model with P-Delta turned off?

RE: column buckling check

Without an initial curvature, this method will not help to find the buckling load.  {F} only contains one element--the one corresponding to axial load.  There's no way for this force to cause moment and corresponding transverse deflection.  Therefore, {Delta} only contains deflections corresponding to axial deformation.

First-order analysis won't give the buckling load using this method because the following system is being solved: [Ke]{Delta}={F}.  Because [Ke] only has material props, section props, and lengths in it, if you increase {F}, then {Delta} MUST increase proportinally.  

Without iterating and moving nodes, the following must be solved: [Ke+Kg]{Delta}={F}  [Kg] has P/L terms if it's linearized and higher order terms if it's geometrically consistent.  This allows non-proportionate {Delta} growth with tiny {F} increases.  This is very, very similar to how AISC's B1 grows as Pr approaches Pe1 in Eq. C2-2.  Pr is analogous to [Kg] and Pe1 is analogous to [Ke].

StrlEIT, try breaking the members up into shorter members.  If Ram uses a linearized Kg, then it's internally overly-restrained which would make it a little stiffer than it should be.  SAP uses a geometrically consistent Kg, so this doesn't happen as much.  I seem to remember that RAM used the goofy linearized Kg.  It's about 10 min. extra effort to use the geometrically consistent one.

RE: column buckling check

Quote:

Any ideas?

Don't use RAM Advanse? I had a bad experience with an oddly shaped truss where RAM Ad was telling me certain web members were zero force. I didn't believe it. Risa3D and RAM Ad were giving very different answers and the Risa3D results seemed to make sense to me. (It wasn't P-delta related.) To this day I still don't know why the difference.

RE: column buckling check

I got it to buckle below 185kips in Advanse by using the Modified Newton Raphson option and adjusting the convergence tolerance to 1.5E-4.  

RE: column buckling check

All -

I'm curious if the RAM guys were ever contacted and asked to explain the differences between their P-Delta results and the other programs.  

It would be interesting to hear what they said. Oftentimes, tech support guys can give a simple explanation for what seems like a very complex difference.  

I find it hard to believe that the average user can be expected to play with convergence tolerances and solution algorithms (Modified Newton Raphson vs what?). That sounds more like what is expected from the users of a true non-linear analysis program.

Josh

PS Disclaimer: My interest is really related to the strengths and weaknesses of various methods of accounting for the P-Delta effect.  I work for another analysis program. We are considering adding an alternate method of P-Delta analysis.  Hence my interest in better understanding the strengths and weakness of the various methods.   

RE: column buckling check

The Ram Advanse user's manual is at http://docs.bentley.com/product.php?prod=204

After reading it, I have no idea why StrlEIT's analysis didn't work or work without tweaking the parameters.  They're using the geometrically consistent [Kg] so that's not it.  They're using element geometric stiffness matrices instead of story-wide matrices, so that should be OK.  I don't see the difference between their description and what SAP2000 does.  Maybe SAP2000's default second-order parameters are better.  I had forgotten that iteration is still required because P in each element might change from iteration to iteration, changing each element's [Kg].

My only guess is that there's something basic wrong with the model, making it stiffer than it should be.

RE: column buckling check

Josh,

How 'bout adding response history analysis?!

100000e

RE: column buckling check

Sorry for the repeated posts, but I just thought of something in the Advanse manual that seems like at least a small booby-trap.  

They do not form [Kg] for shell elements.  Not saying that I know it's wrong, but I'd sure do some careful checking if I had a shearwall structure or was creating a member out of shells to do an analysis similar to StrlEIT's.   

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


Resources