Nonlinear Stability Analysis - Bottom Flange Yielding

[Filip_r]

Hello,

I am currently continuing the development of a nonlinear FE model of a composite steel–concrete perforated beam in RFEM 6 as part of my master’s thesis.

01_OKR_1_3.rf6 (2,7 MB)

I previously created a related topic concerning the concrete Damage model and its deactivation for linear buckling analysis:

Previous Dlubal Community post – RFEM 6: Cannot Deactivate Isotropic Damage Concrete Model for Linear Buckling Analysis

The current question concerns the subsequent nonlinear incremental stability analysis of the same model.

1. Steel perforated beam: S355, surface elements, nonlinear isotropic plastic material model.
2. Concrete slab: C35/45, solid elements, nonlinear anisotropic Damage model.
3. Profiled steel sheeting: S350GD, surface elements, modeled explicitly.
4. Shear connectors: discrete connectors with a nonlinear load–slip (Q–s) relationship.
5. Plate bending theory: Mindlin (surface elements).

The main objective of the analysis is to investigate the behavior and failure mechanisms of the steel perforated beam, especially web-post buckling, local plasticity and the possible development of a plastic mechanism in the bottom flange.

During the nonlinear incremental stability analysis, the calculation currently stops at a load factor of approximately 1.65. At this stage, plastic strains occur mainly locally in the web post, particularly in the region affected by web-post buckling. However, the bottom flange is still almost entirely elastic.

In an earlier model with linear-elastic concrete, the analysis could continue to significantly higher load levels. Yielding of the bottom flange started at approximately a load factor of 1.8.
I have already tested different nonlinear solution approaches, including the post-critical Newton-Raphson method, but the calculation still stops at approximately the same load level. The calculation stops before the maximum number of iterations is reached.

Therefore, I would like to ask:

1. Does RFEM have any internal limitation related to the magnitude, distribution or extent of plastic strains that can terminate a nonlinear incremental stability analysis? Can relatively localized plasticity and web-post buckling reduce the global stiffness of the system sufficiently to prevent RFEM from finding a further equilibrium solution, even if the bottom flange remains almost entirely elastic?
   All user-defined stopping criteria for deformation and plastic strain have been disabled, so the analysis is not being terminated by these limits.

2. In the nonlinear concrete model, I observe very high local compressive stresses in some solid elements, especially close to the shear connectors and load-transfer regions. Could this local behavior and the associated stiffness degradation of the concrete be responsible for the calculation stopping before significant yielding develops in the steel bottom flange?

The profiled steel sheeting is modeled explicitly and acts as the lower reinforcement of the composite slab, while conventional reinforcement is mainly located in the upper part of the slab, but I currently do not model the reinforcement mesh explicitly because the main subject of the study is the steel beam, rather than the detailed behavior of the reinforced concrete slab.

Would the use of a Quast or Modified Quast tension-stiffening model be a reasonable simplified way of accounting for the influence of the upper reinforcement mesh without explicitly modeling the reinforcing bars?
I understand that tension stiffening does not physically replace the reinforcement itself, but I am wondering whether it could provide a sufficiently realistic approximation of the slab stiffness and cracking behavior for a model whose primary purpose is the analysis of the steel perforated beam.

I would be very grateful for any comments regarding the numerical behavior of the model, the interpretation of the nonlinear stability limit, and the simplified modeling of slab reinforcement.

[marc.gebhardt]

Hello Filip_r,

First of all, what a great project!

I'd like to start by going back a bit here. The most important point: It is recommended to test all complex relationships using simplified models. In scientific studies in particular, it is a good idea to even devote a separate chapter to this topic. In the context of your analysis, this applies, for example, to the load-bearing behavior of a sheet metal plate with concrete applied to it. In this case, I would start with a simple surface model and, if necessary, then examine a combined surface-volume model.

Unfortunately, the meshing of your volume elements is far too coarse to accurately represent the nonlinear behavior. Even to correctly calculate the deflection alone, more elements would be needed along the height. Feel free to take a look at this technical article on mesh convergence. To accurately simulate the nonlinear material behavior, the requirements become even more stringent. Please refer to the solution for surface elements, in which the concrete is divided into 15 integration points by default. This is due to the determination of an element’s stiffness. For this purpose, the current stiffness is determined from the material law, which is constant within the element. In a surface element, this is determined at the integration points based on the height. In a volume element, it is determined across the entire element. The following rule of thumb therefore applies: An FE element must be able to represent the desired stress-strain state. Please also note that hexahedrons perform better than tetrahedrons.

As you can see in the next image, even in your static load combination, nearly the whole concrete is damaged under tension. So at the next increment no compression zone is left.

In my opinion, the easiest way is to avoid this and start with surface models. I’ve attached this for you below. ⁣ Here, the calculations are set up according to second-order theory (not large deformation) and the standard Newton-Raphson method (instead of post-critical). In my opinion, this should also be investigated further. I’d also like to offer you one more piece of advice: You’ve set the convergence criteria much more leniently; I can only advise against this, especially to such a high degree. I’ve reset them to the default values. Please also take a look at this knowledge base article.

01_OKR_1_3-surf.rf6 (2.7 MB)

In addition, I included reinforcement in the concrete overlay and took its stiffness into account. The major advantage, aside from a more realistic assessment of the structural behavior of reinforced concrete, is that this also allows you to display the results of the nonlinear reinforced concrete analysis, such as crack widths. You can also apply tension stiffening if you wish. Furthermore, you can also explicitly model the reinforcement via the member-type rebar.

For the fundamentals and modeling in RFEM, I also recommend checking out the webinars and manuals on nonlinear reinforced concrete analysis and nonlinear stability analysis.

One final note: Please also keep in mind that, without further measures, the trapezoidal sheet metal is not shear-rigidly connected to the concrete slab.

If you wish, you can also submit your thesis to us after completion and receive great benefits.

Best regards,
Marc