Greetings,

I am trying to examine local buckling in corroded steel W-Sections in compression. I've modeled this in Solidworks as local section loss and holes in the areas that are corroded. I've tried running both a nonlinear and buckling analyses but neither are giving me very good results. I've also tried subjecting the sections to extremely high loads and exaggerated section loss when I know that local buckling will govern, and the nonlinear analysis does not show any buckling or local deformation around the holes.

Does anyone know if it is possible to analyze local buckling in steel with solidworks, or will I have to resort to a more substantial FEA software package like ABAQUS?

Thanks!

hi andy,

i do not use SW simulation, but most likely the buckling analysis in SW is a linear or eigenvalue buckling which predicts the theoretical buckling of an ideal linear elastic structure. as in your case nonlinearities or imperfections will prevent most structures from achieving theoretical strength and it is not reccommeded to be used for engineering analysis for the real world. linear buckling can be used to help one predict the mode shapes of the structure and the load factors to aid in the modeling for the the more accurate nonlinear buckling, which is a merely a static analysis with large deflection on.

i'll tell you what i know about this and how to perform the analysis as i would using ANSYS. usually most FEA packages use the same approaches with small nuances. as a check, i included my analysis results so perhaps we can compare.

for the nonlinear analysis to predict buckling, a few things need to be done to get the structure to buckle...

first, if the load is in plane or purely axial, the out of plane deflections will not be large enough to intitiate buckling. this is probably why your nonlinear analysis did not show buckling, but merely compression. to initiate buckling, apply a small out of plane temporary force or displacement, this out of plane load should simulate the real world structure as buckling is sensitive to locations/magnitudes of these loads.

second, the load needs to be incremented in small steps. thus if you have a 1000 lb load, perhaps you might want to apply the load 1000 times at 1 lb increments. if the increment is too coarse the buckling load may not be accurate. in ANSYS, turning on automatic time stepping will do just this, increment the load for you until the solution no longer converges. see screen shot of solution progress. you can see when the solution no longer converges, this is the point at which the structure buckles and the corresponding load can be extracted at this point. you merely need to find the load for this time increment and that is your buckling load.

steps for buckling in ANSYS which may or may not be valid in SW sim...

1. run a linear buckling to with a unit load get insight to the failure modes and the buckling load factor.

2. set up a static analysis with large deflection using same geometry as above. use a load larger than the one predicted in step 1 (don't forget to account for gravity loading). remember, you want to load the structure until it buckles, and this will occur when the model convergence fails so have too large a load is ok.

3. if no out of plane or lateral loads exist that will initiate buckling, place them at the locations that will initiate buckling to match the mode shape of interest from step 1. these are loads that should be temporary. in ANSYS i created 2 load steps in the second load step, i turn off the buckling displacement load so as not to interfere with the results.

4. run the model and increment the load until the model no longer converges. in ANSYS, using auto timstepping will automatically increment the load. for this analysis i used a min time step of .0001s and a max of .01s.

i ran the static analysis w/large deflection on (which becomes an iterative nonlinear analysis) and when the solution fails, it occurs at the buckling load. a warning here and that is there could be other reasons why the solution failed such as numerical instability. so check your model for issues before believing the results.

how the buckling load is found...

the nonlinear analysis use an interative solver to increment the load until a solution cannot be found. in ANSYS, if the model does not converge, it will perform a bisection and try again with a smaller time (load) increment, if this converges, then the load is valid and the solver will march forward again until the solution no longer converges and then ANSYS will perform another bisection using a smaller increment (but not smaller than the min increment specified). this occurs until a solution cannot be found and it is at this point the model is buckling. for this case i used a min increment of .0001s and a max of .01s.

screen shot of linear buckling, load factor indicating a buckling load multiplier of 6777 lbs for this slender steel bar of 1"x10"x100".

below is a screen shot of the force convergence showing a solution convergence iterations and number of bisections until the solution failed at approx .677 seconds.

below is the result from the nonlinear buckling. looking at the table in the lower right, you can see the time and the corresponding load. thus in this case, we get the same a slighty more conservative result that the linear buckling

let me know how you make out with your analysis.

best,

dave

If what you are expecting to see is a rippling of the flange on the compression side (ie local buckling or aka crippling) you need to ensure that this mode can show up. In addition to what the last poster responded with (which was pretty good in some respects and it all applies to getting the same result in Simulation- the key thing being that if out of palne forces can not develop on their own from the loading then you need to supply one - math models are geometrically perfect which is what makes you have to be aware of and deal with this issue - alternatively you could displace a node transversely by a thou or two before loading or early on in the loading - it would accomplish the same thing) you need to ensure that you have sufficient elements in the flange to have the mode manifest (I would guess say 4 elements per wave length).

If this was my problem I would do a linear buckling extraction and find out at what load factor the mode you are looking for actually shows up and under what conditions. Most of the standard structural shapes won't manifest crippling before some other mode causes them to fail so it might be a bit tricky to get this to occur. I would develop a model by makig the flanges thin to to explore what it takes to get it to occur under your conditions - my bet is that the local buckling margin is not stronly affected by the imperfections - holes - assuming they are small portions of the area. However you can always do what they do for light standards - they cut holes in the bottom for access and then put in a reinforcing ring with as much material as was removed from the cut out.

Buckling is far trickier than what people typically assume - the Euler buckling of 3rd year mechanics of materials courses is just the start of the story - it gets a lot more complicated quite quickly after that.

Oh, and a couple more things: to get things to go past buckling is a bit tricky numerically which means you typically have to use a control scheme different from force control (which is what the previous poster had used which leads to solution failure prior to buckling - path length (aka arc length or more specifically the Riks or Crissfields method) is the typical choice but displacement control could also work in this particular case if you really neded to get past the instability. The other thing is that a remote load is often convenient to use to get the right BC's at the end where the load is being applied - be aware that it doesn't work properly in a NL analysis. If you are going to rely on a linear buckling estiamte you might want to use a factor of safety of 4 or possibly greater especially if the shape (displacements) under the computed load factor is much different than than the unloaded shape. If a force control NL solution can actually get to the desired load factor for serviceability plus some margin then this would be reassuring.

Thanks very much David and Bill for taking the time to provide such detailed responses, your expertise is greatly appreciated. I really haven't had much experience at all in the past with computer FEA, so it will likely take me awhile to digest (and figure out how to impliment) the numerous tips you have provided me with. Starting with an initial displacement is something I obviously overlooked, and has already helped me obtain more reasonable results.

In response to Anthony and Derek, I am currently doing some preliminary work to try and decide how to impliment an appropriate test in a lab environment. I'm hoping a SW simulation model will help me identify critical flange loss patterns which initiate local buckling in corroded W-shapes in compression. The rig will essentailly consist of a ~2m W-section with simulated corrosion with pin/pin end conditions. I may have a SW model and photos to share in the near future, but not as of yet.

andy,

if you want to upload a model, i'd be happy to run it if it does not becom too involved.

dave

This may be what you are trying to do. Took several minutes to set up. Not sure what you mean by W section. American terminology? In Australia it typically refers to big I sections. Ran the study with and without a small side load. Little variation in buckling load factors. You would need to be a bit more careful about defining the restraints. Anyway this gives an idea of the kind of results you can get using a solid mesh. You still have not stated why you don't think the results were any good.

## Attachments