The simplified upper-bound relationship between tensile stress and displacement used in this research is illustrated in Figure 3. For the CPD model, there are key parameters that must be defined, including (i) the viscosity parameter, which helps smooth out the material response in Abaqus/Standard, and (ii) the dilation angle, ψ, representing the angle of inclination of the failure surface relative to the hydrostatic axis. The dilation angle controls the plastic flow and overall material behavior under loading (Abaqus, 2012).

The different concrete material properties used in ABAQUS Standard, defining materials and step modules, are given in.

Table 1 The elasticity modulus (Ec) of concrete was calculated using the ACI code given by Equation 1. E c = 4700 f c ′ (1)

The CPD model (Abaqus, 2012) initially developed for concrete materials (Abaqus, 2012) is versatile enough to simulate the behavior of other quasi-brittle materials, such as masonry and mortar. This model is designed to capture two primary failure mechanisms: tensile cracking and compressive crushing. The key inputs required for the CDP model are the material’s uniaxial stress-strain behavior under tension and compression (Abaqus, 2012). In tension, the material is assumed to exhibit linear-elastic behavior up to its peak tensile strength, beyond which it follows a softening curve, as illustrated in Figure 4a. In compression, the response begins with a linear elastic phase, transitions to a hardening region, and finally undergoes softening, as depicted in Figure 4b. These behavioural characteristics allow the CDP model (Abaqus, 2012) to accurately represent the progressive damage and nonlinear response of quasi-brittle materials under complex loading conditions.

The main advantage of this material model is its ability to differentiate between tension and compression behaviours, capturing variations in yield strengths, tension softening, and elastic stiffness degradation. In concrete, this stiffness reduction is primarily due to tensile cracking and compressive crushing, as represented by scalar-damage theory. A single scalar damage variable quantifies the extent of damage and modifies the elastic stiffness. The stress-strain relationship, incorporating this damage parameter, is expressed in Equation 2, illustrating the material’s transition from an undamaged to a damaged state. σ = 1 − d · D 0 el / ε − ε pl = D el / ε − ε pl (2) where D 0 e l is the initial undamaged elastic stiffness of the concrete and D e l = (1-d) ∙ D 0 e l is the degraded elastic stiffness of the concrete, and d is the scalar stiffness degradation variable, the range of which is 0 ≤ d ≤ 1, where the value 0 corresponds to undamaged material and one to fully damaged material. The effective stress is defined in Equation 3. σ ¯ = D 0 el / ε − ε pl (3) and is related to the Cauchy stress through the scalar degradation variable as Equation 4. σ ¯ = D 0 el / ε − ε pl (4)

Different parameters, including the dilation angle, define the plasticity model of concrete ψ , the plastic potential eccentricity (ɛ), the ratio of compressive stresses in the biaxial state to the uniaxial state σ b 0 / σ c 0 , shape factor (K_c), and the viscosity parameter. The values of the dilation angle and viscosity parameter were taken from calibration. The yield shape surface (Kc) and eccentricity (ɛ) values are 2/3 and 0.1, respectively, recommended by the concrete damaged plasticity model. The specified value of the stress ratio σ b 0 / σ c 0 , is 1.16 by (Abaqus, 2012) proposed Equation 5 to quantify this stress ratio σ b 0 / σ c 0 based on a large body of statistical data. σ b o σ c o = 1.5 f c ′ − 0.075 (5)

The compressive stress-strain diagram for concrete is shown in Figure 5, according to Eurocode 2 (EC2. Eurocode 2, 2004) According to the ABAQUS manual (Abaqus, 2012) the linear elastic behavior can be taken up to 0.4f _cm (EC2. Eurocode 2, 2004) proposed the approximate relationships built on the experimental results provided by Equations 6, 7 to determine the strain ε_c1 at the average compressive strength of concrete and the ultimate strain ε_cu1. ε c 1 = 0.0014 2 − e − 0.024 f c m − e − 0.140 f c m (6) ε c u 1   = 0.004 − 0.0011 1 − e − 0.0215 f c m (7)

Equation 8 provided by EuroCode 2 (EC2. Eurocode 2, 2004) the research used nonlinear behaviour of structures to model the concrete stress-strain relationship. σ c = f c m k η − η 2 1 + k − 2 η (8)

Where in Equation 9 k = 1.05 E c m ε c l f c m ,   η = ε c ε c l (9)

EuroCode 2 (EC2. Eurocode 2, 2004) also proposed an equation for the non-linear behaviour of the stress-strain relationship of structures, given by Equation 10 σ c = E o ε 1 + ε ε c o 2 (10)

Where, ε_co is compressive strain at peak loads, and according to EuroCode 2 (EC2. Eurocode 2, 2004) is equal to 0.002. EuroCode 2 (EC2. Eurocode 2, 2004) modified the tension-stiffening model of RC given by Figure 6. In this modified model, the only change was that the sudden drop of the tensile stress-strain curve at the critical strain εcr was from the ultimate stress σto to 0.77σto, instead of 0.80σ_to.

The Tensile behaviour of Concrete in ABAQUS was estimated by using Equation 11 (EC2. Eurocode 2, 2004) f t ′ = 0.33 f c ′ (11)

The softening branches in concrete’s compressive and tensile behaviours indicate crushing and cracking. The elastic range is defined by Young’s modulus and Poisson’s ratio, while the inelastic range uses stress-inelastic strain data. Additional plasticity parameters, such as dilation angle, viscosity parameter, stress ratio, eccentricity, and shape factor (K), are needed to accurately describe the material’s plastic behavior (Abaqus, 2012). The dilation angle reflects the material’s internal friction angle and affects shear dilation during plastic deformation. Plastic Potential Eccentricity measures how quickly the hyperbolic flow potential converges, typically set at 0.1. The stress ratio compares compressive yield stress in biaxial and uniaxial states, with a default of 1.16. The shape factor (K) indicates the hydrostatic effective stress ratio between tensile and compressive meridians, affecting the yield surface shape, and ranges from 0.5 to 1, with a default value of 0.667. Lastly, viscosity is a regularization parameter that converges the concrete’s constitutive equations during Abaqus/Standard analyses (Abaqus, 2012), helping ensure numerical stability. These parameters, as summarized in Table 2, are critical for accurately modelling the nonlinear behavior of concrete under various loading conditions.

Figures 7, 8 explain the detailed modeling process of the RC frame in ABAQUS (Abaqus, 2012). The front view of the SSSB is depicted in Figure 7a, while Figure 7b shows the beam-column connection, where the column’s bottom face is the master surface and the beam’s top face is the slave surface. This interaction approach also applies to the connection between the beam and the steel plates in Figure 7c. The RC frame’s support conditions, fixed at the bottom, are illustrated in Figure 7d. A 60 mm thick rigid steel plate was attached to the beam using a 'tie constraint' per ABAQUS standards, with the plates modeled as rigid elements having a Young’s modulus of 210 GPa and a density of 7.85 × 10⁻⁹ ton/mm³. Lateral loading was implemented to maintain the top end of the beam in a free state, thereby ensuring accurate representation of support conditions and load application. This approach guarantees a precise assessment of both support and loading parameters.

Figures 8a–d, illustrates the modelling of the steel cage in the SSSB RC frame. As per the ABAQUS guidelines, the steel mesh should be embedded within the concrete, as shown in Figure 8b. Using this technique, the nodes of the reinforcing bar elements were constrained to maintain compatibility with the degrees of freedom (DOF) of the surrounding host elements (concrete), as depicted in Figure 8c. To evaluate the lateral load-deflection behaviour of the SSSB RC frame up to failure, a static load was applied to the beam’s left side through the displacement control method, by using the Static General option in Abaqus. The displacement increment was set to 10 mm, allowing for a gradual and controlled application of load until structural failure occurred.

The essential parameters for the damage plasticity model of concrete were calibrated using experimental data in conjunction with the Static General Load option in Abaqus. The calibrated values include: (1) viscosity parameter: 0.0028, (2) dilation angle: 38°, (3) shape factor: 0.677, and (4) stress ratio: 1.0, as described in Table 3. A static load was applied until failure, with displacement increments under control. The numerical load-deflection curves for the analysed RC frame were compared with experimental results, confirming that these calibrated values accurately simulate the material’s behavior under load.

The load-deflection curves of the examined reinforced concrete (RC) frame, when compared to those obtained through experiments, indicated the following calibrated parameter values: (1) a viscosity coefficient of 0.0028, (2) a dilation angle measuring 38°, (3) a shape factor of 0.677, and (4) a stress ratio of 1.0. These calibrated parameters were determined based on the results from the control model (CM) tests, as shown in Figures 9 –12.

The calibrated Control Model (CM) was subsequently utilized for the numerical analysis of additional models, as detailed in the following section. Figure 9 illustrates the effect of the viscosity parameter on the columns' load-deflection response. The performance of the viscosity parameter is influenced by the size of the time increment used in the analysis. To achieve optimal results, smaller viscosity parameter values should be evaluated in conjunction with the pseudo-time scale of the finite element analysis. According to (Khan et al., 2020; Saeed et al., 2015; Ahmad et al., 2023; Raza et al., 2021; Ahmad et al., 2021; Raza et al., 2019; Ahmad and Cotsovos, 2023; Ahmad and Raza, 2020; Khan et al., 2015) the time increment step should be approximately 15% of the pseudo-time to ensure greater accuracy. In this study, the time increment step was set to automatic, with both the initial and maximum increment sizes fixed at 0.01 throughout the analysis. The most accurate approximation of the viscosity parameter was 0.0028, selected from the tested values of 0.0018, 0.0028, and 0.0038. This calibration was conducted with the dilation angle held constant at 38° and the mesh size set at 20 mm, ensuring consistency across the simulations and providing reliable results for the numerical modelling.

The dilation angle is a key material parameter for concrete, physically interpreted as the internal friction angle of the material. A sensitivity analysis of the dilation angle was conducted to evaluate its influence on the axial load-deflection response of the control sample. The Drucker–Prager plastic potential function is mathematically defined by Equations 12, 13, where αp represents the dilatancy parameter for concrete. The flow potential function utilized in the CPD model is derived from the Drucker–Prager hyperbolic function (Abaqus, 2012). This function, expressed in Equation 12, is derived from Equation 13. In this formulation, ψ represents the dilation angle, which defines the angle of inclination of the failure surface about the hydrostatic axis. The parameter ε denotes the eccentricity of the plastic flow potential function, which governs the shape of the hyperbolic flow potential curve. G = 2 J 2 + α p I 1 (12)

Additionally, σt0 refers to the uniaxial tensile strength of the concrete at failure. Using the Drucker–Prager plastic potential function, as defined by Lee and Fenves (Abaqus, 2012) in Equation 13, the value of the dilation angle ψ is set to 38. G σ = ε σ t 0 ⁡ tan ⁡ ψ 2 + q ¯ 2 − p ¯ tan ⁡ ψ (13)

In Equation 13, ψ is the dilation angle, ε is the eccentricity of the plastic flow potential function needed to modify the shape of the hyperbola and σ t 0 is uniaxial tensile strength of concrete at failure can be rewritten as Equation 14. G σ = ε σ t 0 ⁡ tan ⁡ ψ 2 + q ¯ 2 + 1 3 I 1 ⁡ tan ⁡ ψ (14)

For the considered range of αp, the dilation angle (ψ) is expected to lie between 31° and 42°. This study analysed dilation angles of 33°, 38°, and 43°.

The results revealed that a dilation angle of 38° provided the best agreement with the experimental data when the viscosity parameter was set to 0.0028, and the mesh size was 20 mm. Consequently, a dilation angle of 38° was selected for all specimens' finite element (FE) simulations. Figure 10 illustrates the influence of the dilation angle on the axial load-axial deformation response for the control model (CM). The load-deflection curves indicate that, although changes in the dilation angle affect the results, their influence is relatively minor compared to the significant effect of the viscosity parameter.

As it is exhibited by Figures 9, 10, the load-displacement curve in relation to viscosity and dilation angle exhibits a comparable trend. This correlation can be attributed to the opposing effects of these variables on one another. During the calibration process, when one parameter is altered, the other remains constant, allowing for a comprehensive examination of the specific impacts involved.

Figure 11 illustrates the impact of different shape factor values, denoted as Kc, on the load-deflection behavior observed in the control specimen. The analysis encompasses three specific Kc values—0.667, 0.9, and 1.0—chosen to represent a range from a lower bound of 0.667 to the upper limit of 1.0. These values were selected to investigate how variations in the shape factor affect the structural response under applied loads, particularly in terms of deflection characteristics. The results indicate that increasing Kc has no significant impact on the load-displacement curve, as illustrated in Figure 11. Consequently, a value of Kc = 0.667 was selected to achieve optimized results while minimizing computational time for the control model (CM).

For the calibration of the Stress ratio, σ b 0 / σ c o (Abaqus, 2012) as shown in Figure 12, the different values 1.0, 1.16, and 1.32 are used. However, all the values exhibited the same results. Thus, the value of 1.0 is used to get the optimized results and analysis time for the CM.

Figure 13 provides a comprehensive visualization of the structural response and failure mechanisms of the SSSB RC Frame at ULS, emphasizing the critical role of material behaviour and damage distribution. Figure 13, numerical predictions derived from finite element analysis conducted using ABAQUS demonstrate the detailed distribution of critical parameters along the span of the SSSB Reinforced Concrete Frame at the ULS;

a. Stress (S33): The distribution of vertical stress (S33) along the span reveals tensile and compressive areas in the concrete frame under load.

The SSSB RC frame serves as the control model in this research due to the wealth of experimental test data available. Initially, flexural cracks were detected near the column bases when horizontal displacement reached approximately 6 mm. As the lateral load increased, additional cracks formed, especially around the connections between beams and columns, revealing significant stress concentrations in those areas. Eventually, diagonal cracks developed in the upper sections of the columns, extending into the beam-column joints. This underscores the progressive damage mechanisms and the susceptibility of these connections when subjected to lateral loading. Furthermore, the DAMAGE figure from ABAQUS is presented in Figure 15c, which compares the Damage with the experimental results and SAP 2000 results.

Figure 14 provides an in-depth view of the reinforcement’s stress and yield characteristics, emphasizing their role in resisting lateral loads and contributing to the specimen’s overall structural performance. Figure 14 Numerical predictions from the ABAQUS (Abaqus, 2012) finite element analysis illustrating the reinforcement behavior in the SSSB RC Frame at the ULS.

a) Axial Yield Criterion (AC Yield) Distribution: This illustrates where the axial yield criterion is met or exceeded in the reinforcement bars, indicating the onset of plastic deformation under load. It highlights critical zones of yielding, essential for evaluating structural capacity and safety.

Figure 15a: This figure illustrates the results of the push-over analysis conducted in SAP 2000 (SAP, 2013), focusing on the formation, location, and classification of plastic hinges in the frame members at the ULS. The plastic hinges are categorized into distinct performance levels B (Barely Yielded), IO (Immediate Occupancy), LS (Life Safety), CP (Collapse Prevention), D (Damaged Beyond Repair), and E (Failure)—providing a detailed depiction of the progressive failure mechanisms within the structure. Figure 15b: This counterpart visualization presents the corresponding predictions from ABAQUS. It offers an alternative perspective by showcasing the extent and severity of damage in the frame members as they approach failure. The ABAQUS (Abaqus, 2012) model captures the structure’s nonlinear behavior with higher fidelity, highlighting stress concentrations and regions of significant plastic deformation.

Figure 16 presents a comparative analysis of the load-deflection curves, showcasing the overall response of RC frames under applied loading as predicted by ABAQUS (Abaqus, 2012) and SAP 2000 (SAP, 2013) and the experimental data obtained during physical testing. The load-deflection curve from SAP2000 consistently predicts a higher load-carrying capacity for the RC frames than what is observed in experiments, highlighting the shortcomings of its modelling method. Conversely, the predictions made by ABAQUS are more in line with experimental results, successfully replicating the structural response under different loading conditions and demonstrating its reliability in modelling the complex behavior of RC frames.

For RC frame analysis (SSSB RC Frame C-SF), modifications have been made to examine the behavior of a modified frame known as HDB. The beams in this modified frame have transverse reinforcement that is half the size of the stirrups used in the control model. As a result, as shown in Table 4, the transverse reinforcement in the beams is reduced by 75% compared to the original frame that was experimentally studied. The transverse reinforcement arrangement in the modified frame under consideration is shown in Figure 17.

Figure 18 comprehensively illustrates the structural response of the HDB with reduced transverse reinforcement, emphasizing its impact on stress distribution, damage patterns, and failure mechanisms. Figure 18 described the stress (S33), strain distribution (E33), compressive damage (DAMAGEC), plastic equivalent strain (PEMAG), and their contour damage distribution in the modified specimen HDB at the ULS.

Figure 19 provides an in-depth view of the reinforcement’s stress and yield characteristics, emphasizing their role in resisting lateral loads and contributing to the specimen’s overall structural performance. The analysis presents numerical predictions of AC Yield and Maximum Principal Stress (S, Max) from ABAQUS for the Half Diameter of Stirrups in Beam (HDB) model at ULS. It reveals stress distribution and deformation patterns in reinforcement elements, emphasizing critical areas where materials approach capacity. This visualization illustrates how a reduced stirrup diameter affects the beam’s structural integrity and load resistance under extreme conditions, offering insights into the performance of reinforced concrete components at failure.

Figure 20 provide a comparative analysis of the structural behavior of the modified Half Diameter of Stirrups in the Beam (HDB) model, as predicted by SAP2000 and ABAQUS. Together, these figures underscore the differences in predictive accuracy and detail between ABAQUS (Abaqus, 2012) and SAP 2000 (SAP, 2013) offering a comprehensive understanding of the structural response and damage mechanisms in the modified HDB model under extreme loading conditions.

Figure 21 offers a comparative evaluation of the load-deflection behaviour derived from experimental data and computational simulations. This comparison highlights the accuracy and reliability of the modelling techniques used to capture the structural response of the control specimen, providing insights into the applicability of each approach.

To investigate the behavior of the RC frame with reduced transverse reinforcement, the Half Diameter of Stirrups in the Beam and Columns (HDBC) model was analyzed in comparison to the Control Model (CM), as outlined in Table 4. This modification results in a 75% reduction in transverse reinforcement in both the beams and columns compared to the original frame tested experimentally. A significant reduction in stirrup dimensions was implemented to assess its impact on structural performance, particularly in terms of load-carrying capacity, ductility, and damage progression. Figure 22 illustrates the transverse reinforcement details for the modified frame, including the updated configurations and reduced dimensions. These adjustments highlight the impact of transverse reinforcement on the structural behavior under loading conditions, providing a clear contrast between the CM and HDBC models. This comparison offers valuable insights into the critical role of stirrups in maintaining the stability and integrity of RC frames under applied loads.

Figure 23 comprehensively illustrates the structural response of the HDBC with reduced transverse reinforcement, emphasizing its impact on stress distribution, damage patterns, and failure mechanisms. Figure 23 described the stress (S33), strain distribution (E33), compressive damage (DAMAGEC), equivalent strain (PEMAG), and the contours of these values in the modified HDBC at the ULS.

Figure 24 provides an in-depth view of the reinforcement’s stress and yield characteristics, emphasizing their role in resisting lateral loads and contributing to the specimen’s overall structural performance. Figure 24 describes the axial yield criterion (AC Yield), Maximum Principal Stress (S, Max), and numerical predictions from the ABAQUS finite element analysis, which illustrate the reinforcement behaviour in the HDBC at the ULS.

Figures 25, 26 present a ABAQUS (Abaqus, 2012) and SAP 2000 (SAP, 2013) comparative analysis of the predictions obtained from SAP2000 and ABAQUS for the modified HDBC frame. The analysis reveals that SAP 2000 (SAP, 2013) tends to overestimate the load-carrying capacity of the modified frame compared to the predictions provided by ABAQUS (Abaqus, 2012). This observation highlights differences in the modelling and computational approaches of the two software tools.

To investigate the behavior of the RC frame, increasing the spacing of the stirrups twice in beams and columns as DSBC, the model was analyzed in comparison to the CM as outlined in Table 4. This modification results in a 50% reduction in transverse reinforcement in both the beams and columns compared to the original frame tested experimentally. A significant reduction in stirrup dimensions was implemented to assess its impact on structural performance, particularly in terms of load-carrying capacity, ductility, and damage progression. Figure 27 illustrates the transverse reinforcement details for the modified frame, including the updated configurations and reduced dimensions. These adjustments highlight the impact of transverse reinforcement on the structural behavior under loading conditions, providing a clear contrast between the CM and DSBC models. This comparison offers valuable insights into the critical role of stirrups in maintaining the stability and integrity of RC frames under applied loads.

Figure 28 comprehensively illustrates the DSBC’s structural response to reduced transverse reinforcement, emphasizing its impact on stress distribution, damage patterns, and failure mechanisms. Figure 28 described the stress (S33), strain distribution (E33), compressive damage (DAMAGEC), plastic equivalent strain (PEMAG), and contours of these values distribution in the modified DSBC at the ULS.

Figure 29 provides an in-depth view of the reinforcement’s stress and yield characteristics, emphasizing their role in resisting lateral loads and contributing to the specimen’s overall structural performance. Figure 29 describes the axial yield criterion (AC Yield), Maximum Principal Stress (S, Max), and numerical predictions from the ABAQUS finite element analysis illustrating the reinforcement behaviour in the HDBC at the ULS.

Figures 30, 31 present a comparative analysis of predictions obtained from ABAQUS (Abaqus, 2012) and SAP 2000 (SAP, 2013) for the modified DSBC frame. The comparison reveals that SAP2000 overestimates the modified frame’s load-carrying capacity compared to ABAQUS. This highlights differences in the computational methodologies and structural behavior predictions of the two tools for the modified DSBC frame.

Figure 32 illustrates the comparison of lateral displacements by encompassing (i) experimental results, (ii) ABAQUS (Abaqus, 2012), and (iii) SAP-2000 (SAP, 2013) for the four case studies mentioned above, i.e., (a) CM, (b) HDB, (c) HDBC, and (d) DSBC. The experimental results are only available for the CM configuration, showing a lateral displacement of approximately 60 mm, whereas no experimental data is reported for HDB, HDBC, and DSBC.

In the numerical simulations, ABAQUS shows varying lateral displacements, with the CM model reaching 30 mm, while other configurations (HDB, HDBC, DSBC) exhibit lower values. This indicates ABAQUS’s sensitivity to material properties and boundary conditions. In contrast, SAP results display uniform lateral displacements of 90 mm across all configurations, suggesting insensitivity to material variations or oversimplifications in modelling. Notably, the experimental displacement for the CM configuration is significantly higher than the predictions from both ABAQUS and SAP 2000, indicating challenges in accurately capturing real-world structural behavior in numerical simulations. In summary, while the numerical tools offer valuable insights, the consistency in SAP-2000 results and discrepancies from experimental data highlight the need for improved modelling. Furthermore, validating all configurations experimentally is crucial for enhancing reliability and strengthening the correlation between experimental and simulation results.

Figure 33 illustration compares lateral load across (i) experimental results, (ii) ABAQUS, and (iii) SAP-2000 for four case studies: (a) CM, (b) HDB, (c) HDBC, and (d) DSBC. Experimental data is only available for the CM configuration, which shows a lateral load of approximately 60 kN. The lack of data for HDB, HDBC, and DSBC limits validation of the numerical simulations. ABAQUS shows varying lateral load capacities, with HDB having the highest load, followed closely by CM; HDBC and DSBC exhibit slightly lower values. This indicates ABAQUS’s sensitivity to material properties and boundary conditions. In contrast, SAP-2000 displays a uniform lateral load of 90 kN across all configurations, suggesting that it may not effectively capture material-specific variations. The difference between the experimental load for the CM configuration and the numerical predictions from ABAQUS and SAP-2000 suggests limitations in the simulation models, which may not fully capture real-world conditions, such as imperfections and nonlinearities. While numerical simulations provide insights into structural performance, the consistent results from SAP, combined with the lack of experimental data for certain configurations, underscore the need for validation across all setups. Additionally, improving modelling strategies in numerical tools could enhance predictive accuracy. The FEA model, HDB, shows a 10.2% increase in lateral load compared to CM, while HDBC and DSBC exhibit discrepancies of −15.8% and −15.5%, respectively, compared to the experimental values.