Numerical model development and validation

An advanced numerical model is developed in ANSYS 15.0 [47] finite element program. The model is based on a full shell model using four-node-thin (SHELL181) and eight-node-thin (SHELL281) shell elements with linear and with serendipity base functions, respectively. Two analysis types are applied, geometrical nonlinear buckling analysis (GNBA) for the determination of the critical load amplifier and geometrical and material nonlinear imperfect analysis (GMNIA) for the determination of the ultimate resistances. The applied numerical model can handle the application of residual stresses, measured initial geometric imperfections as well as equivalent geometric imperfections. Fig. 18a presents the developed geometrical model with the boundary and loading conditions. The numerical model is simply supported and the compression flange is constrained against lateral displacement to ignore lateral torsional buckling. The bending moments are applied in the flanges through force pairs at both ends.

a) geometric model b) material model

Fig. 18: Applied geometric and material model.

A linear elastic - hardening plastic material model with von Mises yield criterion is used in the numerical model. The material model behaves linear elastic up to the yield stress (fy) by obeying Hook’s law with Young’s modulus equal to 210000 MPa shown by Fig. 18b. The yield plateau is modeled up to 1% strains with a small increase in the stresses. By exceeding the yield strength the material model has an isotropic hardening behavior with a hardening modulus until it reaches the

29

ultimate strength (fu). From this point the material is assumed to behave as perfectly plastic. In the validation procedure of the FE model the measured yield and ultimate strengths are implemented for all the tested girders, in the numerical parametric study, however, the nominal yield and ultimate strengths are applied relevant for S355 steel grade.

2.5.2 Convergence study

Mesh sensitivity analysis is executed to study the applicable element type and number of finite elements per fold length to ensure high accuracy in the numerical modeling. In addition, member length dependence study is also performed in order to give a limit number how many corrugation waves are needed as a minimum to analyze, in order to ensure the accuracy of the critical stress from GNB analysis. Fig. 19 presents the result of the convergence study of the GMNI analysis using four-node (SHELL181, blue lines) and eight-node (SHELL281, red lines) shell elements.

a) specimen 9TP3 (cf/tf≈12) b) specimen 4TP2-2 (cf/tf≈22) Fig. 19: Results of the convergence study for the ultimate resistance.

The vertical axes represent the ratio of the numerical and test based resistances and the horizontal axes demonstrate the number of applied elements per fold length. The same tendencies are observed whether equivalent geometric imperfections using the first eigenmode shape are applied in the FE model or no imperfections are applied (e.g. the blue curves tend to the corresponding red curves). It can be observed that in the case of eight-node-shell elements (SHELL281) 4 elements along the fold lengths could be acceptable in average due to its fast convergence, while 6-10 elements are needed to reach acceptable accuracy, if four-node-shell elements (SHELL181) are applied.

Fig. 20 presents the results of the convergence study for the GNB analysis. The vertical axes represent the critical load factors normalized to their investigated minimum values (αcr,6 – 6 elements over one fold). The horizontal axes represent the applied element numbers along the fold length. The results reveal that in the case of SHELL281 4 elements within the fold length is judged

30

to be acceptable. Therefore, this element type is used in the following calculations having at least 4 elements along the web fold.

a) specimen 9TP3 (cf/tf≈12) b) specimen 4TP2-2 (cf/tf≈22) Fig. 20: Results of the convergence study for the critical bending moment.

Fig. 21 shows the results of the convergence study in the function of the member length for four different flange width-to-corrugation depth ratios (bf/a3). The vertical axis represents the critical load amplifier depending on the number of the analyzed wave length.

Fig. 21: Convergence study on the member length.

It can be observed that by using flange width-to-corrugation depth ratio equal or smaller than 5, the number of the minimum wave lengths to be analyzed is two, in order to eliminate the effect of the end supports from the critical load amplifier. For larger bf/a3 ratios, however, at least 4 corrugation waves should be modeled. Therefore, in the current numerical parametric study the minimum number of the applied corrugation waves are larger than 4. These considerations are applied in the design of the test specimens presented in Section 2.4.

2.5.3 Numerical model validation

In the frame of the experimental research program the initial geometric imperfections of the compression flanges and the strains in the tension flanges are measured. All the measurements are presented in Section 2.4. These results are used to validate the current numerical model. Fig. 22a shows the schematic drawing of the applied residual stress distribution predicted from the strain

31

gauge measurements on the test specimens in accordance with the proposal of Watanabe and Masahiro [26] and Lho et al. [42]. Fig. 22b presents the defined longitudinal stress distribution in the FE model. After defining the residual stresses the equilibrium stress state is calculated as shown in Fig. 22c.

a) schematic model b) defined residual stresses c) equilibrium situation Fig. 22: Longitudinal residual stress distribution.

Fig. 23: Actual collapse mode and ultimate shape from the numerical simulation (4TP2-2).

This equilibrium residual stress distribution is applied in the GMNI analysis including the measured actual initial geometric imperfections of the compression flange. The process of the FE model validation is shown in Fig. 23 in the case of specimen 4TP2-2. The geometrical and material properties of each specimen according to their numbering can be found in Section 2.4.2. Before the loading tests, 11 specimens’ initial geometric imperfections are measured and applied in the numerical model. It has to be noted that by applying the above described initial imperfections in the numerical simulations, similar failure modes and ultimate resistances are observed in the

32

numerical model than measured in the laboratory tests. The results of the numerical model validation are summarized in Table 5 where the first and second columns show the specimen numbers and the large outstand-to-thickness ratio (cf/tf).

Table 5: Numerical model validation by the test results.

Number cf/tf Mtest

[kNm]

Mnum,geo

[kNm]

Mnum,geo+res

[kNm] Mnum,geo/Mtest Mnum,geo+res/Mtest

1TP1-2 20.0 322.7 370.0 342.9 1.15 1.06

2TP1-1 20.2 369.1 413.3 381.5 1.12 1.03

2TP1-2 20.2 364.8 404.6 376.3 1.11 1.03

3TP1-2 11.0 739.9 717.1 716.3 0.97 0.97

4TP2-2 22.5 289.2 323.9 300.7 1.12 1.04

5TP2-2 22.8 321.3 367.0 340.0 1.14 1.06

6TP2-2 12.1 740.7 730.5 728.4 0.99 0.98

7TP1 13.1 587.7 571.5 568.7 0.97 0.97

8TP2 14.2 550.1 546.3 540.1 0.99 0.98

9TP3 12.0 585.0 576.2 575.5 0.99 0.98

10TP4 13.0 571.5 569.9 564.7 1.00 0.99

The columns #3, #4 and #5 represent the ultimate bending moment resistances measured in the tests, computed by the FE simulations with applying only the initial geometric imperfections and calculated by FE simulations with both initial geometric imperfections and residual stresses, respectively. The ratios of the FEM based and test based resistances are included in columns six and seven. It can be observed that in the case of very slender flanges having cf/tf ratios larger than 20, the residual stresses have significant effect on the load carrying capacities (specimens 1TP1-2, 2TP1-X, 4TP2-2, 5TP2-2). The resistance differences are obtained to 8-9% which may confirm the results of Li et al. [27] where the differences are obtained to 5% for cf/tf ≈17 and 14% for cf/tf≥24.5.

It can be seen that by applying the initial geometric imperfection and the residual stresses in the FE model the structural behavior follows the actual behavior observed in the tests. It is proved by the comparison of the failure modes and the bending moment resistances as well. The statistics show that the average deviation is obtained to be 1% with a coefficient of variation equal to 0.034 and with a maximum deviation equal to 6% for slender flanges.