The nonlinear analysis of reactive powder concrete effectiveness in shear for reinforced concrete deep beams

2.1 Material modeling

In any numerical study, the simulation of any model under applied loads depends on the behavior and mechanical properties taken from the structural material used in construction. Different materials from which reinforced concrete members can be built (normal or reactive powder) concrete and steel will take collective behavior as a uniting rule. The stress–strain relationship will be similar in tension and compression when steel will be considered a homogeneous material.

On the contrary, the stress and tension behavior of concrete is different, as it is a heterogeneous semi-brittle material because its internal mixture is mainly dependent on the properties of all its mixtures. The RPC is cement mortar, steel fiber, silica fume, and air voids. The efficiency and accuracy of a computer model depend mainly on the appropriate modeling of material properties [15].

2.2 Numerical simulation of deep beams using ABAQUS

Considering the outlay of money and time involved, RC deep beam reactive concrete behaviors include many parameters: load–displacement response, crack pattern, mode of fraction, and the ultimate strength of concrete. Moreover, the numerical investigation of the lattice variability of the models by 50, 25, and 15 in terms of the running time, the maximum concrete strength, crack pattern, and mode of failure cannot be completely understood, and obtained by laboratory validation. Moreover, the numerical study can add information about RPC deep beams of shearing behavior. But the limitations of numerical analysis cannot fully solve the desired problem. Therefore, numerical analysis along with empirical validations is necessary for further study of the behavior of reinforced deep beams with RPC type.

The simulation of RPC-type reinforced deep beams was studied by ABAQUS software V20.0 using an advanced numerical model [16]. This research will study the behavior of non-linear concrete under compression and tension. The concrete damaged plasticity model from ABAQUS software was used to define the materials and extract data on stress and inelastic strain, which will be used as main inputs in the program to calculate other parameters such as the maximum shear strength and displacement in the compression and tensile regions of the concrete. Simulation data acquisition was evaluated using laboratory data that included two deep beam samples with the same dimensions (500 mm × 150 mm × 1200 mm) and the shear extent to effective depth ratio of 0.774 with the use of a four-point loading system for the reference and RPC deep beam.

2.3 Material properties

Accurate data on the mechanical properties of any material is an important key factor in any numerical analysis. The data obtained through the model’s simulation were compared with the data obtained with the previous experimental new research and the maximum error was kept less than or equal to 6%. The mechanical properties of normal concrete, RPC, and steel used to simulate the models in this research article are explained in Table 1.

Moreover, in the present simulation, the actual modulus of elasticity was computed based on ASTM C42/C42M-18a (drill core test) [17] The proposed stress–strain curve calculation was performed to select the uniaxial stress–strain values in the studies of Desayi and Krishnan and Gere and Timoshenko [18,19]. Using relationships and some equations, the damage coefficients for compression and tension behavior are calculated by Lubliner et al. and Lee and Fenves [20,21]. Plasticity will be the flow parameter as shown in Table 2.

For compression damage, in ABAQUS, the user provides the d _c– ε c in data.

Depending on ABAQUS user manual will internally compute the plastic strain [21,22] as follows:

where ε c pl is the plastic strain in the compression damage; ε c in is the inelastic strain in compression damage, which can be computed by ε c in = ε c – ε 0 c el ; ε _c is the compressive strain, which can be computed by the cylinder test (compressive test); ε 0 c el is the elastic strain in compression damage, which can be computed by ε 0 c el = σ c E 0 ; and d _c is the damage parameter in compression damage, which can be deduced from the mechanical properties of the material with sloping loading/unloading cycles as follows:

where σ _i is the compressive stress at any point in the stress–strain curve; σ _cu is the maximum compressive stress (i.e., crushing point), which can be deduced from the stress–strain curve; and E ₀ is the initial modulus of elasticity for the material which the slope over the stress–strain curve.

Finally, it will obtain the value of plastic stress in compressive damage ( ε c pl ) from the earlier equation and check that the value is positive and that it always increases with inelastic stress.

For tension damage, in ABAQUS, the user provides the d t – ε t in data and, with the same earlier steps that calculated the plastic strain for compression damage, the plastic strain for tension damage will be calculated.

where ε t pl is the plastic strain in the tension damage; ε t ck is the cracking strain in the tension damage, which can be computed as follows:

ε _t is the tensile strain, which can be computed by the splitting tensile test (based on ASTM C496); ε 0t el is the elastic strain in compression damage, which can be computed by ε 0t el = σ t E 0 ; d _t is the damage parameter in the tension damage, which can be deduced from the mechanical properties of the material with sloping loading/unloading cycles as follows:

σ _i is the tensile stress at any point in the stress–strain curve; and σ _tu is the maximum tensile stress (i.e., crushing point), which can be deduced from the stress–strain curve.

Finally, we deduce the plastic strain in the tension damage ( ε t pl ) from the earlier equation and check that it is all positive and that it is always increasing with the cracking strain. During the simulation, any increase will result in a new damage variable. It is extracted based on the maximum difference between the value of the previous increase in the end and the current data of the stage in contrast. For concrete, the tensile behavior of failure is linear and beyond; the formation of microcracks is described microscopically using the results of the stress–strain diagram. Concrete damage plasticity (CDP) values in compression and tension damage are shown in Tables 3–6. The final summary of data for both RC deep beams with and without RPC are yield stress and inelastic strain are used in ABAQUS. These data are computed by using analytical equations suggested in the ABAQUS analysis user manual [16].

2.4 Constitutive models

2.4.3 Solid element

For linear and complex nonlinear analyses in the ABAQUS program, solid elements can be used, including contact, plasticity, and large distortions. For the numerical simulation presented in this article, the C3D8 – Bricks is used to model deep beam concrete and loading plates and endurance. The abbreviation represented by the term is shown in Figure 2 [23].

Figure 2

Abbreviation of the term C3D8.

2.4.4 Truss element

Other essential elements of this research are reinforcement rods for longitudinal reinforcement. Reinforcing bars are important for transmitting natural forces. For this, reinforcing bars in the form of three-dimensional gear elements are sufficient. The T3D2 – Truss is used to model the reinforcing rods in the numerical simulation of deep beam specimens. The abbreviation represented by the term is shown in Figure 3 [23].

Figure 3

Abbreviation of the term T3D2.

2.4.5 Meshing

To get accurate data from the finite element (FE) model, the model containing all the elements will intentionally allocate the same mesh size to ensure that in the same node two different materials will share it. For the modeling of concrete, loading, and support plates, the mesh element will be an eight-node brick element with three degrees of freedom of translation at each node (C3D8). In this article, three sizes of meshing were used (50, 25, 15), and the results were verified in terms of running time and maximum applied load. Figure 4 shows the typical mesh of a deep beam sampling numerical simulation model. Mesh and modeling generation were optimized using the same techniques for all specimens.

Figure 4

3-D meshing of deep beam concrete model in ABAQUS.

2.4.6 Loads and boundary conditions

For constraining the model and for a unique solution, the displacement boundary conditions will be needed. Constraints are put on a single line of nodes on the board in the UY and UX directions. The support case is shown in Figure 3. The force, P, is applied to the steel plate across the entire center line of the plate. Figure 5 shows the plate and the applied load.

Figure 5

Boundary conditions at support and applied load on the model.

3.1 Load–deflection responses

For ABAQUS, displacements were computed at the same position. As for the numerical models, the mid-distance deviations were measured in the middle of the bottom face of the specimens and the experimental data were investigated and the following notes were made.

1. The numerical data for displacement were in good agreement with the laboratory data when the error rate did not exceed 10%.

2. We notice that the curve of the concrete deep beam (CDB) reference beam and the RPC deep beam (RPCDB) in the experimental work drops sharply from the top of the highest applied load while the decline in the finite element analysis is diagonal and less severe.

3. The deflection rate increased more at the maximum loads while the models showed an increase in the displacement rate close to the final load.

4. In terms of stiffness, the load–displacement numerical curves were always relatively higher and slightly higher compared to the corresponding experimental curves. The numerical and experimental load-mid span deflection curves are shown in Figures 6 and 7.

Figure 6

Load–displacement curve for reference deep beam (normal concrete) between experimental and FEA.

Figure 7

Load–displacement curve for deep beam (RPC) between experimental and FEA.

3.2 Numerical ultimate shear load

The results of the finite element analysis (FEA) of the maximum loads which the given element to the pilot loads corresponding deduced in Table 7 for deep beams and the following notes are inserted and implemented.

1. Through numerical simulation, we note that the maximum expected load obtained from ABAQUS software showed good agreement with the experimental data when the error rate did not exceed 10%.

2. For most of the beams, the maximum shear load in the numerical simulation was emphasized concentrically on the experimental data by 2% for the normal CDB and 5% for the RPCDB.

3. The numerical simulation reduced the strength of the deep beams by 2–3%. One reason for this difference was that the crack faces have reinforcement mechanisms which may also very slightly increase the failure of the lab beams before the complete collapse. The numerical simulation of the models had no such options.

4. To compare the beam carrying capacity, the finite element models had the same sequence as the actual beams. Comparison of the numerical results for CDB resulted in a 2% maximum load enhancement, with respect to reference deep beam CDB.

5. Comparison of the numerical results of RPCDB resulted in a maximum load enhancement of 5% with respect to the experimental RPCDB beam.

3.3 Radial crack load and crushing patterns

Through the data obtained from the numerical simulation using the ABAQUS program, we notice an increase in the radial crushing load when the load was gradually increased, where the crack seemed clear going from the support to the load point. The radial crushing load obtained from the laboratory results was lower than that taken out from the ABAQUS data by 2% for the normal CDB and 5% for the RPCDB. The difference between the ABAQUS data and the laboratory data was because of the comparison of the relative fit of the numerical simulation models with the relative covariance of the real beams. Using ABAQUS software, the crack patterns in each applied loading step have been recorded as shown in Figures 6 and 7, and these charts show the evolution of the crack patterns for each specimen. When the applied load became high, the appearance of tensile cracks was observed, and when the applied loads began to gradually increase, there were many radial cracks and additional bending; then compression cracks appeared when the applied load reached the final stages of failure [24].

For the two deep beams tested, the failure mode was as predicted. The laboratory deep beams that failed are documented by taking out pictures and the crack patterns are accurately determined to be then compared with numerical simulation models during the incremental loading phases. As for the CDB reference beam, by using ABAQUS software, the crack patterns for numerical simulation models and experimental beams have been well examined and studied. Through the experiment and examination in this research article, it has been observed that the radial shear cracks extend from the support toward the load point. The high shear stress region has been observed to have many cracks. The crack pattern at failure mode from the experimental work and simulation by the ABAQUS program of the deep beam of CBD can be observed in Figure 6. The comparison shows the same behavior where vertical cracks (flexural cracks) are observed at mid-span followed by the development of diagonal cracks within the critical shear region at the left and right side of the shear span of the beam.

Moreover, the shear cracks started close to the center of support as in laboratory work and gave a good validation for FEA that can help to use this software to make the new designation in the future for other variables such as shear span to effective depth ratio. Finally, the failure mode and crack pattern of the deep beam for a four-point load shows homogeneity depending on the crack distribution for both sides of the deep beam as experimental work.

A radial concrete tensile failure or splitting failure occurred in a reference beam and was a radial crack that formed at each shear interval from the inner edge of the support toward the inner edge of the point load. A diagonal crack extended above the diagonal line between the center lines of the point loads and the supports, and it is mentioned in Figure 8.

Figure 8

(a) Experimental crack pattern, (b) FEM-crack pattern, and (c) FEM-mode failure for deep beam (CDB).

It has been observed that the deep beam (RPCDB) has a very common failure mode, which is the shear compression failure. Shear compression failure has been described in the flexural compressive zone by cracking concrete at the tip of the main radial notch. The flexural compression zone was characterized by the extension of the main radial crack from the inner face of the support towards the inner face of the loading point. In this article, we note that the failure in the deep beams occurred suddenly without warning, and the movement would fail and extend along the oblique fissure. Figure 9 mentions a typical shear-compression failure.

Figure 9

(a) Experimental specimen, (b) FEM-Crack pattern, and (c) FEM-mode failure for deep beam (RPCDB).

3.4 Mesh changing effect

In this article, the mesh of the models was changed to three sizes (50, 25, 15) and this change was studied in terms of the maximum applied load and the time required to complete the simulation of the models. It has been observed that when the network size is reduced, the maximum applied load will also be reduced. The reference specimen CDB was taken as a model to observe the change of the mesh. The effect of the mesh changing is shown in Figures 10 and 11.

Figure 10

Changing mesh for control deep beam CDB.

Figure 11

Comparison between the different meshing for control deep beam CDB.

It was noted that with the changing of mesh size of the reference model to 50, 25, and 15, it will require a running time of 16, 100, and 438 min, respectively. As for the maximum numerical shear load at a mesh size of 50, it was noticed that it increased by 2.27% compared to the shear load for experimental work. On the other hand, the numerical shear load decreased at sizes 25 and 15 by 16 and 30.4%, respectively, compared to the shear load for the previous experimental work. It is important to note that the finite element analysis study is approximate in nature due to several factors, the most important of which are [25] the following:

1. An approximation in material simulation related to concrete and steel plate.

2. An approximation was inherent in the simulation of the numerical model’s technique.

3. An approximation is used in the integral function in numerical simulation.

4. The approximation was presented due to the type of implementation option used to solve the nonlinear system of equations.

3.5 Dimension changing effect

In this article, the dimensions of the model were changed to an overall length of 1,700 mm, a depth of 400 mm, and a thickness of 150 mm, and this change was studied in terms of the maximum applied load, crack pattern, and mode of failure to complete the model simulation. The CDB and RPCDB models were taken as models to monitor the effect of dimensional change. The effect of changing dimensions is shown in Figure 12 and Table 8.

Figure 12

(a) FEM-crack pattern (CDB), (b) FEM-mode failure (CDB), (c) FEM-crack pattern (RPCDB), and (d) FEM-mode failure (RPCDB).

It was observed that the maximum shear load increased by 15% for the reference model CDB when increasing the dimensions of the model, while there was an increase in the maximum displacement by 29%.

As for the RPC model (RPCDB), there was a decrease in the value of the maximum shear load by 11%. On the contrary, there was an increase in the maximum displacement by 12%.

For the reference model (CDB) with new dimensions, where the shear crack pattern was densely spread and extended from the support to the point load, and the mode of failure was a shear-compression failure, while the model with the old dimensions, the shear cracks were limited and extended from the support to the supporting load and mode of failure was a shear failure. The RPC (RPCDB) model with new dimensions was also similar to CDB in terms of the crack pattern and mode failure.