3D-ABAQUS Modelling of Prestressed Concrete Hunched Beams with Multi-Openings of Different Shapes

A long-span Prestressed Concrete Hunched Beam with Multi-Opening has been developed as an alternative to steel structural elements. The commercial finite element package ABAQUS/CAE version 2019 has been utilized. This article has presented the results of three-dimensional numerical simulations investigating the flexural behaviour of existing experimental work of supported Prestressed Concrete Hunched Beams with multiple openings of varying shapes under static monotonic loads. Insertion openings in such a beam lead to concentrate stresses at the corners of these openings; as a result, extensive cracking would appear. Correlation between numerical models and empirical work has also been discussed regarding load displacement and crack development, and the obtained outcomes demonstrate a good agreement with the experiments. The ratio of ultimate loads and deflection of the beams tested in the investigation to those of numerical models was 0.98 and 0.97, respectively. So, finite element analysis can be regarded as a behaviour-trustworthy technique for simulating the non-linear behaviour of prestressed concrete rafters with multi-openings from the point of view of complexity, hardly, time-keeping, human effort, and cost.


INTRODUCTION
The advantages of Prestressed Concrete Hunched Beams (PCHBs) in industrial and bridge buildings, structural portal frames, and framed structures have been frequently utilized (Hou et al., 2015). Instead of prismatic beams, these beams minimize the structure's weight, allowing for larger spans with no apparent reduction in loading capabilities (Naik et al., 2017). Researchers began looking for perforated RC rafters in the early sixties. (Salam et al., 1977;Mansur et al., 1991). Insertion openings in this type of beam have various advantages, including arithmetic flexibility, ease of shipment, and the construction of a structure where service pieces of machinery can pass during the web of beams, and, most importantly, the decrease in overall weight. Concrete is also relatively inexpensive and has good fire resistance (Abdulkareem et al., 2022). It's also low-maintenance to support the roofs of warehouses, industrial facilities, and aeroplane hangars instead of steel parts (Hassan et al., 2019a;Alkhafaji et al., 2020). On the other hand, insertion openings in such a beam lead to concentrate stresses at the corners of these openings; as a result, extensive cracking would appear (Hassan et al., 2019b;Tu'ma et al., 2021), which is unacceptable from both aesthetics and durability standpoints. Consequently, the beam would be less rigid, leading to excessive deflections while under service loads. Because of this, the design of these beams need special treatment to keep the crack width under control and prevent the beam from failing prematurely (Mansur et al., 1999;Sahi et al., 2021). Since concrete lacks significant tensile strength, creating long-span beams is challenging. To bypass this problem, prestressed reinforcement was required, as achieving the required span lengths with ordinary reinforcement was impossible (Samir et al., 2013;Al-Hilali et al., 2022a). Al-Hilali and others investigated the short-term deflection of prestressed concrete hunched beams with various opening configurations (Al -Hilali et al., 2022b). The parametrical examinations of this research were the opening configurations (quadrilateral or circle) and the chord depths. It was found that specimens with round holes were stiffer when loaded than those with trapezoidal holes. Furthermore, rafters with inclined posts and trapezoidal holes were stiffer than beams with vertical posts. They examine the performance of prestressed concrete hunched beams with multi-openings of different shapes PCHB systems by conducting a numerical analysis of a commercial version of ABAQUS/CAE 2019. This is a flexible analysis tool that may be used to address both linear and non-linear problems. Additionally, ABAQUS is a robust numerical gadget often used for modelling. But the performance of concrete is sophisticated, and several factors must be considered for analysis, in which concrete experiences stiffness degradation and strain-softening in both compression and tension (Lubinar et al., 1989). The ABAQUS software's Concrete Damage Plasticity Model (CDPM) has been introduced to fit the earlier behaviour of concrete and other quasi-brittle materials. The degradation process in the elastic stiffness is expressed in the damage parameters and , illustrated in Fig. 1 for compression and tension, respectively. Under a four-point load, nine regular concrete beams with openings, five high-strength concrete beams with openings, and one beam as a reference solid with normal concrete were evaluated. The most important discovery was that the ultimate strength decreased, and cracking was enlarged in normal concrete beams when the diameter of the aperture surpassed one-third of the beam's depth. This was the case in all of the beams tested. At the same time, the diameter and the position of the aperture are the primary parameters that influence the strength of the concrete. Later, (Al-Shaarbaf et al., 2007) introduced a three-dimensional "Finite Element Model" that can simulate the flexural behaviour of concrete beams with only one rectangular opening. Validation was carried out using numerous models, including a rectangular transverse opening demonstrating a good agreement between the experimental and numerical findings. The significant factors studied on the structural behaviour of the member were the concrete strength, reinforcing ratio, and opening size. Ultimate strength and post-cracking stiffness for beams increased when the amount of bottom reinforcement and the concrete strength increased but decreased with increasing opening size. (Madkour et al., 2007) suggested a modern theory of non-linear three-dimensional elastic damage to model the deformation of the reinforced concrete (RC) beam. The simulation of the non-linear behaviour of RC beams with openings based on thermodynamics was given more attention. The non-linear elastic behavior and the degraded condition of concrete materials are taken into account in the suggested theoretical method. The provided non-linear concrete model has been validated using a series of numerical simulations of experiments analyzing the behaviour of reinforced concrete beams subjected to monotonic static loads. The experimental data presented in the literature were compared with the suggested model, and a good agreement was found. To comprehend the behavior of concrete, several researchers have constructed constitutive models (Park and Paulay, 1975;Scott et al., 1982;Wang and Hsu, 2001;Seow and Swaddiwudhipong, 2005). But although there are many of these methods, several areas still need further investigation. Based on the input information, notably the material properties, finite element (FE) software may perform a realistic analysis of structures. Concrete is widely utilized in the construction industry, although it is highly non-linear under uniaxial compression as a composite material. As a result of its brittle behaviour. So, Concrete fails to crack under tension and crushes under compression. Concrete failure modelling has become a concern in modern concrete structures. This study investigates the serviceability (deformability and cracking) Of Perforated Prestressed Concrete Haunched Beams (PPCHBs) subjected to external concentrated load at mid-span. Adopting this work finds the optimum model of PPCHBs depending on the correlation between the covered variables, namely: number, size, the configuration of the openings, and inclination of the posts, and the maximum load-carrying capacity.

Geometrical Modeling
Describing the geometric elements of the tested specimen is the beginning stage in finite element modelling. Fig. 2 depicts the finite element idealization for the tested beam under static loading, which includes all beam components.

Material Modeling
Under all stress states, excluding the hydrostatic pressure, concrete experiences stiffness degradation and strain-softening in compression and tension (Lubinar et al., 1989). The Concrete Damage Plasticity Model (CDPM) in the Abaqus software has been introduced to fit the earlier behaviour of concrete and other quasi-brittle materials. The degradation process in the elastic stiffness is expressed in the damage parameters and , illustrated in Fig. 1 for compression and tension, respectively. The damage parameters are complicated to be mathematically expressed. (1), and no damage occurs in the stiffness before the apex of the stress-strain curve.
where; is the stress in concrete (N/m 2 ), is the ultimate stress (N/m 2 ), and the subscripts and refer to compression and tension, respectively. In tension, = . This formula is used in the current study to evaluate and define the damage parameters (compression deformation) and (tensile deformation). To determine the plasticity characteristics of concrete, the (CDPM) model needs five plasticity parameters, primarily: 1. Dilation angle ( ): it is the internal friction angle of the material or, in other words, the increase in concrete's plastic volume is more than the value of critical stress. (ABAQUS User Manual, 2013). As a rule of thumb, = 20° to 40° is suggested in simulations, which affects the material's flexibility. As a result, the dilation angle profoundly impacted the entire model. An increase in the dilation angle increased the system's flexibility.

4.
Parameter: the ratio of the second stress invariant on the tensile meridian, ( ), to that on the compressive meridian, ( ). The default value is 2/3 was adopted in this research. 5. The viscoplastic regularization parameter ( ): is a parameter that is necessary for the viscoplastic regularization of the model. This parameter improved the model's convergence rate during softening, resulting in favourable outcomes. In the present study, the value of μ = 0.0004 was adopted.

Compressive Behavior of Concrete
Uniaxial compressive behaviour can be defined by an existing constitutive model proposed by (Hognestad, 1951) (i.e., the stress-strain relationship of concrete), as shown in Fig. 3 and suggested in Eq. (2), which has been adopted in this simulation.
where; σ c nominal concrete compressive stress (MPa). E c : Modulus of elasticity of concrete (MPa). ⸍ : Maximum compressive strength of concrete (the unconfined cylinder specimen) (MPa). : nominal compressive strain in concrete. : Strain at maximum stress (the strain at the curve's peak point). From beginning to end, the equation for the non-linear behaviour of concrete was assumed.
Damage caused by increased plastic strains in semi-brittle materials is shown as a reduction in the curve's tangent concerning the initial diamond (modulus of elasticity, ), as seen in Fig. 1. At the curve's apex (i.e., ultimate compressive stress ⸍ ), the damage parameter ( ) was zero; then, it gradually decreased to 0.8, concerning 20% remaining strength in big strain. (Hafezolghorani et al., 2017).

Tensile Behavior of Concrete
Concrete subjected to tension is not regarded as a brittle-elastic form, and such phenomena as aggregate interlocking inside cracks and concrete-steel adhesion amidst cracks are considered. Therefore, the stress-strain drop in the tension zone does not occur suddenly but is relatively progressive. The Finite Element (FE) analysis results for RC concrete structures are highly sensitive to the user-defined parameters of tension stiffening. These parameters are the ultimate tensile stress and ultimate cracking strain. The post-failure strain softening of the tensile stress demonstrated in Fig. 1b can be approximated to linearly vary from the maximum tensile stress ( ) at failure strain ( , ) to zero at the ultimate total cracking strain ( ). Thus, ( ) is the total cracking strain at which a complete loss of tensile strength is reached. According to (Reddiar, 2010), this strain is one-tenth that corresponding in compression ( ), and is evaluated according to Eq. (4): when; ⸍ = 45 MPa, for instance, will be 7.5 × 10 −4 . While this value, according to estimating (Abaqus analysis user's manual,2013) about 10 × 10 −4 . The inelastic cracking strain ( ) that should be defined as not the total strain but after deducing the failure strain ( / ). Again, the manual suggests starting the analysis with a failure strain of 1 × 10 −4 . Hence, the ultimate will be 7.5 × 10 −4 ; it is 7.5-times , . The ultimate cracking strain adopted in the current modelling is taken equal to 7.5 As mentioned in the ABAQUS analysis user manual, increasing the values of the tension stiffening parameters enables FE solutions. In contrast, using too few values results in a local cracking failure, which causes unstable behaviour. The input data (material properties) for concrete with the CDPM were carried out in tabular format, as shown in Table 1.

Reinforcement Steel Modeling Properties
The reinforcements and stirrups steel has been modelled numerically as elastic-perfectly plastic depending on the von mises failure, which considers the material elastic behaviour up to the yield stresses and, after this point, becomes completely plastic, as shown in Fig. 4 (ABAQUS User Manual, 2013). The modulus of elasticity and Poisson's ratio of the reinforcement material are the two factors that determine the linear isotropic portion, which has been taken as 200×10³ MPa, and 0.3, respectively. As presented in the experimental test, the bilinear isotropic portion is defined via yield stress. Also, the steel bearing and support plates are simulated as linear isotropic substances. The reinforcement material uses the same values to simulate linear isotropic for both the modulus of elasticity and Poisson's ratios 200×10³ MPa and 0.3, respectively. The prestressing steel was modelled as multilinear isotropic material. The modulus of elasticity of the strand and Poisson's ratio are 197.5×10³ MPa and 0.3, respectively.

Load Application and Boundary Conditions
In the simulation, the boundary conditions and the external load application were identical to those utilized in the experimental tests. One of the support structures was represented as a hinge, while the other was modelled as a roller. (Ux=Uy=Uz=0) was used to ensure the constraining of one of the supports and act as the hinge. And it permitted longitudinal displacements and rotations toward the x-axis while simultaneously restricting the y and z directions (Uy=Uz=0), achieving modelled roller support, see Fig. 5. The numerical model was initially subjected to the recorded prestressing strand force in a solitary step of loading (step No.1). The effective stress for the strand was used as the pressure applied in the xdirection during the prestressing process utilizing a predefined field. The tested beam's selfweight wasn't considered, while in (step No.2) of modelling, The load was added to the steel loading plate in the second step. The mesh module includes tools that allow the creation of meshes on the parts and assemblies that have been formed. Many available elements in ABAQUS software can be utilized, and choosing the appropriate element that suits the problem well is essential. The non-prismatic perforated prestressed concrete beams (NPPCBs) are modelled in 3D stress elements for all model components except steel reinforcements, which utilize standard 2D features. These elements provide appropriate integration standards based on the empirical response of the specimen. The maximum approximate size was 20 mm for concrete meshing, 40mm for end and support plates, and 40 mm for reinforcements (mild steel and tendons). The reinforcement steel may be simulated by solid or truss elements. The solid elements are complex arithmetically, so they are not chosen. Since reinforcement bars don't have a high flexural stiffer, truss elements, have been used and modelled as embedded elements, and their bond to concrete is to be completely bonded. Linear brick hexahedral C3D8R elements are continuum elements (C) having 3D eight nodes (8) with reduced integration (R) and were selected for the finite element models for concrete beam, support plates, end bearing plates, and strand volumes. In comparison, T3D2 elements are element (T) having 2D two nodes (2) were selected for the finite element models for Steel reinforcing bars (longitudinal and shear reinforcement). Fig. 6 and Table 3 show T3D2 and C3D8R elements.

EXPERIMENTAL STUDY AND DETAILS OF THE TESTED BEAMS
This section briefly explains the experiment works, including the tested setup and some important conclusions. Details of the empirical study have been published in other publications (Al-Hilali et al., 2022b). Six prestressed concrete hunched beams with multi openings of different configurations and one control specimen (i.e., solid) as a standard beam under monotonic static loading mid-span till failure. A variable that was considered was the number of openings and their height. The tested beams had the same type, size, and dimensions, with a total span of 3000 mm and an exact clear length of 2850 mm. The depth of the mid-span beam is 400 mm, while the depth of the end-section beam is 250 mm (i.e., the depth of the beams diminished as they approached the support). The web width for the beam was 100 mm, the width of the flange was 200 mm, and the depth of the flange was 50 mm. The openings are identified by posts that are 100 mm wide. Figs. 1 and 2 show that the necessary reinforcement details included short stirrups in chords, additional diagonal bars around openings, the posts, and full-depth stirrups next to openings and prestressing strands. Based on the variables, specimens have been divided into three groups (A, B, and C), as seen in Table 5. The materials properties utilized in this study are summarized in Table 6. Cement, coarseaggregate, and fine-aggregate were tested in accordance with Iraqi standards (IQS), whereas mild steel reinforcement was tested in accordance with ASTM standards. They were using a 7-wire strand with a 0.5 (in) diameter (Grade 270), and a post-tensioning jacking force of (110kN) was supplied from one end in accordance with the requirements of ACI-318M-19.  Note: Results represent the average of three control specimens.

PRESENTING AND DISCUSSING THE OUTPUTS OF NUMERICAL ANALYSIS.
The results of the experiments on the tested beams were used as a verification problem and then compared to the numerical analysis outcomes for all tested specimens. In FEM analysis, all of the models use static analysis. Fig. 8 shows the Stress component at the integration point shape of one of the beams that have been analyzed. Table 7 compares the tested beams' camber at mid-span obtained from the experimental work and the finite element model at the prestressing force transfer. Good agreement was obtained between the camber of numerical models and found experimentally where the value of the average and coefficient of variation for ( ) FE. / ( ) Ex was (0.89) and (8.6) %, respectively. Based on the results of the FE analysis, it may be seen that the simulated models are stiffer than the tested experimental results. Several factors could cause the FEM analysis results to show a higher stiffness. During the experiment, Microcracks cracks were found in the concrete, caused by drying shrinkage and treating environmental conditions. These factors would make the actual specimens less stiff. There is no way to model these microcracks cracks in finite element models. In a finite element analysis, an ideal bond is assumed to exist between the concrete and the steel reinforcing. The actual specimen will not wholly match this assumption. The composite work between the concrete and steel reinforcement is lost when a bond slip occurs. This means the FE analysis's predicted stiffness may be higher than the actual specimen's total stiffness (Kmiecik et al., 2011). Fig.  9 shows the shape of one of the camber in a beam that has been analyzed.

Loads and Deflection at the Ultimate Stage
The numerical model addresses concrete's most basic phenomena based on the modified Mohr-Coulomb models. It was established to probe the impact of damage caused by mechanisms of failure in the substance. Table 8 compares the ultimate loads, the deflection at mid-span produced using the FE model, and the empirical works done at the final phase for all tested beams subjected to static testing. There was a good agreement between numerical simulations' failure loads, maximum displacement, and empirically tested outcomes. With the mean value and C.O.V for maximum loads ( ) / ( ) being 0.98 and 2.34%, respectively, and the average value and coefficient of variation for mid-span deflection ( / ) being 0.97 and 6.43%, respectively. Fig. 10 shows the shape of one of the displacement distributions in a beam that has been analyzed.

Load-Deflection
For ABAQUS, the deflections for the experimental beams are recorded at mid-span. The loaddeflection curves obtained from the finite element analyses are compared with the experimental results for test beams, as seen in Fig. 11. Figure 11. Experimental and numerical load-deflection comparison for the analyzed beams.
It can be noticed that the experimental and numerical load-deflection curves have a similar trend and pretty well with the experimental data for all tested beams, however, the loaddeflection responses of the finite element studies for all beams are significantly more rigid than those of the experimental results and for the same reasons mentioned in section 4.1.

Crack Pattern
Based on the CDPM theory, cracks in RC elements are generally formed in regions where the tensile strain occurs exceeds the limited tensile strain in concrete (i.e., the plastic stress for concrete exceeds zero). Therefore (DAMAGE T) damage in tension was utilized as a substitution for crack growth in the flexural zone in the current study. The cracks' orientation is perpendicular to the utmost main plastic strain. In general, diagonal tensile cracks at the corners of the openings occurred early. When the applied loads increased, vertical tension cracks spread along the lower chord, and flexural cracks appeared; this can be monitored in ABAQUS software by navigating between the increments in the second step from loading. analyzed simulation to the crack patterns of the empirical works for tested specimens at the final stage; this depicts the impact of apertures on stress concentrations and the formation of cracks. Based on these figures, stress concentrations occurred at the corners of the apertures and the lower tension chords. Also, an excellent coincidental crack pattern between the numerical and experimental work can be observed.

Stress Distribution along the Beams' Main Reinforcement
The stresses in the longitudinal primary reinforcement (steel and tendon) at the tension chord are shown in Fig. 17 for the three phases of loadings (40 KN, 80 KN, and ultimate loads).

CONCLUSIONS
This work presents a damage plasticity model (CDPM) as a numerical non-linear FE to simulate existing non-prismatic prestressed concrete beams with different shapes of multiopenings. The tested specimens were numerically validated until a satisfactory degree of precision was reached by realizing a good FE modelling technique and entirely accurate material modes. Accordingly, the following conclusions can be drawn:  The CDPM model was an appropriate method to simulate concrete tension cracking and crushing. So, 3D non-linear FE models were developed to evaluate the RC elements' efficacy with the CDPM model. All potential nonlinearities, namely materials and geometrics, were considered in the created FE model.
 The 3D nonlinearity FEM described was then used to model multi-openings of different shapes for prestressed concrete hunched beams. The FE model successfully estimated failure load, the concrete crack growth caused by tension, the stress in steel reinforcement, and mid-span deflection in the prestressed concrete beams.
 The average ratios of loads and displacement at failure between experimentally tested rafters and simulations models were 0.98 and 0.97, respectively. The outcomes indicate that the FE models, when acted with a suitable FE modelling technique and accurate constitutive substance model, are highly successful in representing the nonlinearity behaviour of prestressed concrete hunched beams with different shapes of multiopenings.