*3.1. Global Analysis*

The given design of the structure was recreated in a compatible computer aided design (CAD) format and was imported into the commercial finite element software mentioned above. The finite element model was used to simulate some assumptions and certain loading conditions with a consideration of geometric nonlinearities. The boundary conditions were defined as appropriate to the actual structure and the loads applied to the truss roof system were defined as given in Table 2, which are greater than the loads that are assumed for the design. So, the main purpose of this global analysis was to generate a better understanding of the mechanical behaviour of the roof and to predict the failure modes under different loads and assumptions. It is worthy of note that all the analyses were run in a static manner. Since the equivalent static loads are determined using the relevant Turkish standards, it is appropriate to use this simplification [8].


**Table 2.** The loads considered in the analyses.

One of the most important aspects here is that the presented strength and elastic properties of the materials and members used were put through tests and experimental processes and were found to be consistent in general with the standards [8]. So, in the analyses performed for this study, the values that were presented in the reports of the company were mainly used.

Different dead, live, snow, temperature, and earthquake loads were considered in the design. Rain load caused by an excessive accumulation of water, especially on low-slope or flat roofs where the parapets are mounted around the roof, can cause partial or total destruction if they are not considered in the design. However" rainfall ponding on the roof is considered in the design. The design code used gives wind loads for buildings of 20–90 m tall as 0.8 kN/m<sup>2</sup> (pressure) on the windward and −0.4 kN/m<sup>2</sup> (suction) on the leeward sides. For the seismic loads, the earthquake acceleration is taken as 0.3 g, where g is the gravitational acceleration, so the earthquake loads are overestimated [8].

The loads acting on the space truss system are to be transmitted to the bars over the spherical steel elements, called nodes. The weight of the space truss roof system is taken as 140 N/m<sup>2</sup> , the dead load from coatings and the installation is given in the design documents as 240 N/m<sup>2</sup> , but it was assumed to be 350 N/m<sup>2</sup> in the analysis. The snow load is given in the design calculations as 1000 N/m<sup>2</sup> and was taken as 2000 N/m<sup>2</sup> in the analysis. The equivalent earthquake horizontal load is given as 180 N/m<sup>2</sup> in the design calculations and was considered here as 200 N/m<sup>2</sup> . The equivalent earthquake vertical load was 950 N/m<sup>2</sup> and the vertical wind load was 960 N/m<sup>2</sup> . Table 2 gives the loads used in the analyses.

The boundary conditions of the space truss system and the columns were arranged as the original design of the structure.

The bars of the space truss were modelled based on the standards of DIN S235 JR for quality linear elastic materials, and columns were modelled as C35 grade homogeneous and linear elastic steel-reinforced concrete with the elasticity modulus, which was determined using the homogenisation of the composite column analysis. The bar elements in the space truss system and the beam elements in the columns were assembled as a whole system of 160,133 elements and 461,847 nodes. Figure 6 displays the model for global analysis in a commercial finite element software. With this model, a static global analysis of the space truss system was performed with the above-mentioned loads being quite a bit larger than the design loads.

165

**Figure 6.** Three-dimensional finite element model prepared for finite element (FE) analysis.

## *3.2. Analysis of the Columns and Supports*

This section covers the analyses performed to gain more insights into the mechanical behaviour of the columns and the supports, which either were not very accurately represented in the global model or to increase the accuracy of the global model. The first stage of these analyses aimed to homogenise the composite column and the second stage investigates the mechanical behaviour of the column and support behaviour focusing on the stress/strength of the structure.

#### 3.2.1. Analysis of the Steel-Reinforced Columns

The main purpose of this analysis was to understand the effective material properties of the steel-reinforced concrete columns by using three-dimensional finite elements. Here, the column was assumed to be a composite beam and its material properties were calculated with homogenisation. Thus, the aim was to obtain a more realistic global model. For this purpose, a model was created considering the steel reinforcement of the concrete columns. In this model, the column material was considered as a composite material with concrete and reinforcing steel rods. The steel rods were placed in the concrete as shown in Figure 7. The rods and the concrete were rigidly bonded to each other. According to the general theory of mechanics of composite materials, lateral reinforcement steel binders, which are predicted to have no significant effect on axial stiffness, were not included in the analysis for the sake of simplicity. The steel reinforcing rods were taken as given in the project and as described in the previous section.

To represent the behaviour, a cross-sectional face was subjected to axial displacement restrictions whereas the opposite face, which is the other cross-sectional face, was subjected to a uniform axial displacement. Using the results of the analysis, the effective Poisson's ratio and Young's modulus were determined. A similar procedure was also performed for the effective thermal expansion coefficient. The results of this analysis were used in the global analysis.

μ

**Figure 7.** CAD of a column with steel-reinforced concrete.

3.2.2. Analysis of the Spherical Support with Steel-Reinforced Columns

This part of the study was interested in the mechanical behaviour and safety of the column and spherical support structures. This study used the highest mechanical loads acting on a single truss-column connection node calculated in the global analysis. It is also important to note that this analysis considered only the mechanical loads and did not consider any thermal effects. The analysis of the column support connection was performed with a three-dimensional finite element model.

The column support connection was built such that the sphere was mounted on the support plate, which is embedded in the steel-reinforced concrete with a bolt connection. The structure of this model is given in Figure 8.

**Figure 8.** CAD of the column support connection with steel-reinforced concrete.

The contact interfaces between the steel rods and concrete were rigidly bonded and so too were the contact surfaces between the spherical support and the steel plate. The bolts were attached to the model with a standard preload and connected to the steel plate and concrete with friction.

The bottom cross-sectional face was connected to a grounded spring with 6 degrees of freedom and with the stiffness values of the rest of the column, to save computational time.
