Buckling failure

[hrtuwair]

Hello dears,
I am trying to model a four-point loading test for hollow-rectangular beam made from GFRP. I build the model in ABAQUS and defined almost everything for the analysis except the failure mode I got from the experimental. This beam failed due to buckling of the webs but don’t know how to define this in my model. Any advices please.

Regards

 

[RPstress]

If it is just that you don't know how to ask Abaqus how to do a buckling run you may need to get more basic help, or ask a more specialized forum.

If you are unsure what options to use for buckling of composites then it's easiest to do a linear static eigenvalue-type run with implicit FE. More accuracy can be got with better nonlinear implicit FE or with explicit FE (Abaqus is capable of sophisticated nonlinear implicit or very accurate explicit types of FEA), but it's usually simplest to start out with linear static eigenvalues. It's usual to use layered 2D shell elements. To check the FE results hand analysis can be done with smeared properties found from classical laminate theory equivalent plate properties. If Ex = Ey and Gxy = Ex/(2+2*nuxy) within about 10% it's ok to to use buckling formulas for isotropic material, but if your laminate is more orthotropic than quasi-isotropic then better formulas for composite plates and the like are available, e.g. AFWAL-TR-85-3069, "Buckling of Laminated Composite Plates and Shell Panels" and many others can be found through Google.

Note: the FE should give an option to enter through-thickness shear stiffnesses in the 23 and 13 directions. There is often some argument about these. A reasonably safe initial approach is to make 13 and 23 the same as the 12 G value if the reinforcement is glass. The 23 and 13 values can be reduced by up to about 0.8 times as a check. The 'correct' value to use is usually documented somewhere in your organization's procedures or possibly in the FEA guideance.

If the FE gives buckling loads within about a factor of 1.5 or even 2.0 compared with the hand checks then it's probably about right. Be sure that the buckled shapes shown are reasonable to the eye. Just because it's composite doesn't usually mean any wildly different behavior. The through-thickness shear flexibiliity should make fairly small differences. If your structure is quite complicated then it may pay to get the FE working with some simpler geometry first (a simply supported plate is an old favorite to check). If you've got a fairly thin laminate compared with the ply thickness then the ply sequence could give a marked difference from the hand calcs. The classical laminate bending properties compared with the in-plane ones can give a clue about effects from this. Also if you've got any asymmetry in the laminate then it can give answers that differ more from the hand calcs. You can get an idea of this from NASA Technical Paper 3659 "Buckling Behavior of Long Symmetrically Laminated Plates Subjected to Shear and Linearly Varying Axial Edge Loads".

Ah, I've just read your post correctly and you've got some test results. The above techniques might give some some clues about discrepancies between the FEA and test. While tests can be badly designed the test result is almost certainly the gold standard to be approached by the FEA.