ANSYS program has been used by many researchers for FE modeling of reinforced concrete structures. With regards to FRP strengthened reinforced concrete structures, Kachlakev et al. (2001) used ANSYS to examine the structural behavior of beams and bridges strengthened with FRP laminates. In their numerical modeling, SOLID65, LINK8 and SOLID46 elements were used to model concrete, bars and FRP laminates, respectively. Alhaddad et al. (2012) presented a detailed procedure for nonlinear finiteelement analysis of FRP and textile reinforced mortar (TRM) upgraded reinforced concrete beam–column exterior joints using ANSYS. In their numerical modelling, they used similar elements to those used in Kachlakev et al. (2001). The FE results were compared with the test results through load–displacement behavior, ultimate loads, and crack pattern. Comparison of FE results with the experimentally observed response indicated that the proposed nonlinear FE model can accurately predict the behavior and response of tested RC beam–column joints. Parvin and Granata (2000) investigated the application of FRP laminates to exterior beam–column joints in order to increase their moment capacity using numerical analysis performed by ANSYS. In their study again SOLID65, LINK8 and SOLID46 elements were used to simulate the concrete, rebar and the FRP laminates, respectively. Mahini and Ronagh (2011) investigated the effectiveness of FRP strengthening in relocating the plastic hinge away from the face of the column in beam–column joints.
A quick literature review on finite element analysis of reinforced concrete structures strengthened by FRP laminates shows that the majority of researchers have used SOLID65, LINK8 and SOLID46 to model concrete, rebar and FRP. There are some exceptions though; Hawileh et al. (2012) recently used the ANSYS program to simulate reinforced concrete beams externally strengthened with shortlength CFRP plates. SOLID65 and LINK8 elements were used to model concrete and rebar. On the other hand, instead of using SOILD46 to model the FRP laminates, they used SHELL99 element with orthotropic material properties. Mirmiran et al. (2000) developed a nonlinear finite element model for the analysis of FRP confined concrete. SOLID65 was used to model concrete while the FRP sheets were modelled by tensiononly SHELL41 elements. Their model showed the same type of stress concentration around the edges of square sections as observed in the experiments. Furthermore, they concluded that the cyclic analysis of FRPconfined concrete confirmed capability of the model to effectively predict the cyclic response of FRPconfined concrete. There has not been any study that explores the suitability of the elements in a comparative way; and therefore, this is the target the current study is aiming for.
Concrete
In ANSYS, the only element that is suitable for modeling concrete is SOLID65. This element is used for 3D modeling of solids with or without rebar. The solid is capable of cracking in tension and crushing in compression. The element is defined by eight nodes having three degrees of freedom at each node: translations in x, y and z directions. Figure 3 shows the geometry of element SOLID65. Up to three different rebar specifications can be defined as smeared reinforcement (uniformly distributed reinforcement defined as rebar percentage in each direction using rebar cross section area and spacing). SOILD65 element is capable of plastic deformations as well as creep.
ANSYS uses WilliamWarnke (1974) failure criterion for assessing the state of failure. This failure surface function has five parameters. These parameters are used to find the tensile and compressive meridians. The five parameters that are required to define the WilliamWarnke failure surface are:

f
_{
t
}
:

Ultimate uniaxial tensile strength

f
_{
c
}
:

Ultimate uniaxial compressive strength

f
_{
cb
}
:

Ultimate biaxial compressive strength

f
_{
1
}
:

Confined triaxial compressive strength (compressive meridian)

f
_{
2
}
:

Confined triaxial compressive strength (tensile meridian)
While the full five input parameters are needed to define the failure surface (as well as an ambient hydrostatic stress state on which parameters f_{
1
} and f_{
2
} are based), ANSYS can build the failure surface with a minimum of two constants that are the uniaxial tensile and compressive strengths. For the rest of the parameters, ANSYS uses default values taken from the William et al. (1974) study.
It should be noted that ANSYS treats WilliamWarnke function as a failure surface. Prior to failure, the behavior is elastic, and after cracking or crushing, the material completely fails at that point and the material stiffness suddenly drops to zero. In the case of having pure tension, ANSYS uses Rankin failure criteria for tension cutoff. Cracking is permitted in three orthogonal directions at each integration point. For the direction in which cracking occurs, tensile strength essentially becomes zero. When the crack closes, compressive stresses normal to the crack can be transferred. Material property for the directions in which crack has not occurred remains the same. Figure 4a shows the failure surface of concrete for the plane stress case. As is seen, for the tension stress state, ANSYS uses tension cutoff.
With regards to the concrete tension model, one of the shortcomings of ANSYS is that it does not use the concept of fracture energy which is widely used in the analytical models for concrete cracking. In ANSYS, cracking is defined by a single material property which is the tensile strength of concrete. To consider tension stiffening, stress relaxation has to be considered after cracking. Figure 4b shows the model employed in ANSYS to consider tension stiffening. A constant T_{
c
} is used to control the stiffening model which acts as a multiplier for the stress relaxation.
Shear behavior of SOLID65 element in ANSYS is controlled by two shear transfer coefficient for open and closed cracks. These coefficients represent conditions at the crack allowing for the possibility of shear sliding across the crack face. The value of these shear transfer coefficient ranges between zero and one, with zero representing a smooth crack (complete loss of shear transfer) and one (no loss of shear transfer).
Even though prior to failure (cracking or crushing), the behavior is assumed to be linear elastic, plasticity and/or creep may be combined with the concrete base properties to provide nonlinear behavior prior to failure. Usually, VonMises or Drucker–Prager (Drucker et al. 1952) plasticity is used for concrete. When a yield criterion is used in conjunction with the failure criteria, the yield surface must lay inside the concrete failure surface; otherwise, no yielding will occur. Drucker–Prager yield criterion is a modification of the VonMises criterion that accounts for the influence of the hydrostatic stress component; the higher is the hydrostatic stress (confinement pressure), the higher would be the yield strength. Equations 1 and 2 show the yield functions for VonMises and Drucker–Prager yield surfaces.
\sqrt{{J}_{2}}{\mathit{\sigma}}_{y}=0
(1)
\mathit{\beta}{I}_{1}+\sqrt{{J}_{2}}{\mathit{\sigma}}_{y}=0
(2)
where, parameters β and σ_{
y
} are the yield function parameters or material constants. Figure 5 shows both of the aforementioned yield criteria in the stress invariant plane. The VonMises function depends on only one stress invariant and does not include the effect of hydrostatic stresses, while Drucker–Prager includes the effect of hydrostatic stresses by adding another stress invariant.
Since the Drucker–Prager yield surface is a smooth version of the Mohr–Columb yield surface, it is often expressed in terms of the cohesion c and the angle of internal friction \mathit{\varphi} that are used to describe the Mohr–Columb yield surface. If it is assumed that the Drucker–Prager yield surface inscribes the Mohr–Columb yield surface, then the expressions for finding parameters β and {\mathit{\sigma}}_{y} will be as follows.
\mathit{\beta}=\frac{2\mathrm{sin}\mathit{\varphi}}{\sqrt{3}(3\mathrm{sin}\mathit{\varphi})}
(3)
{\mathit{\sigma}}_{y}=\frac{6(c)\mathrm{cos}\mathit{\varphi}}{\sqrt{3}(3\mathrm{sin}\mathit{\varphi})}
(4)
where in Eqs. 3 and 4, \mathit{\varphi} is the angle of internal friction and c is the cohesion value. The cohesion and the angle of internal friction for concrete are related to the concrete strength as shown in Eqs. 5 and 6.
{f}_{c0}=\frac{2(c)\mathrm{cos}\mathit{\varphi}}{3\mathrm{sin}\mathit{\varphi}}
(5)
{k}_{1}=\frac{1+\mathrm{sin}\mathit{\varphi}}{1\mathrm{sin}\mathit{\varphi}}
(6)
where variable {f}_{c0}^{\prime} is the unconfined strength of concrete and the parameter k_{1} is the confinement effectiveness factor. Confinement effectiveness factor was first suggested as 4.1 by Richart (1929). It results in a friction angle of about 37°. Others have suggested different expressions for calculating this factor. Rochette (1996) suggested a direct approach to calculate c and \mathit{\varphi} as given by Eqs. 7 and 8.
\mathit{\varphi}={\mathrm{sin}}^{1}\left[\frac{3}{1+1.592332{f}_{c0}^{\prime}(\mathit{ksi})}\right]
(7)
c(\mathit{psi})=({f}_{c0}^{\prime}(\mathit{psi})1256)\frac{3\mathrm{sin}\mathit{\varphi}}{6\mathrm{cos}\mathit{\varphi}}
(8)
The internal friction angle and cohesion shown in Eqs. 8 and 9 were used by other researchers (Mirmiran et al. 2000; Shahawy et al. 2000).
In order to simulate the nonlinear behavior of concrete, VonMises yield criterion could be used instead of Drucker–Prager. Equation 9 shows the parabolic function of Hognestad stress–strain curve. Postpeak behavior of concrete involves strain softening. Several softening models are available for concrete. However, in the implicit version of ANSYS, softening of material could not be considered. In this study, the softening branch of stress–strain curve is replaced by a plateau.
{f}_{c}={f}_{c}^{\prime}[\frac{2{\mathit{\epsilon}}_{c}}{0.002}{\left(\frac{{\mathit{\epsilon}}_{c}}{0.002}\right)}^{2}]
(9)
Steel Rebar
There are two options to model the reinforcement bars in ANSYS; smeared and discrete. When the smeared option is used, reinforcement is defined as a part of SOLID65 concrete element. Up to three directions could be used to define the smeared bars. Figure 3 shows the arrangement of reinforcing bars in the element. The smeared rebar is capable of tension and compression, but not shear. In each direction, smeared bars behave similar to a uniaxial material. The second option for modeling the reinforcing bars is to model them as a discrete element which is attached to the concrete elements. If discrete reinforcements are to be modeled, use of LINK and COMBIN elements in ANSYS is suggested; amongst which 2node uniaxial tension–compression LINK8 element is the most common. As previously mentioned, VonMises yield criterion is generally used for metals such as steel. Steel can be modeled as a bilinear or a multilinear material. For cyclic analysis, generally one of the more common Kinematic hardening laws is used for the rebar. In the current study, bilinear Kinematic material behavior is used for bars. Longitudinal bars of beams and columns are modeled using discrete LINK8 element, but the shear bars (stirrup) are modeled using smeared reinforcement. Because no bond slip was reported in the Mahini’s (2005) experimental study in the current research bond elements are not modeled.
Fiber Reinforced Polymer (FRP)
FRP composites are anisotropic; that is, their properties are different in different directions. A schematic of FRP composites is shown in Fig. 6. As is seen, the unidirectional lamina has three orthogonal planes of material properties (i.e., x–y, x–z, and y–z planes). The xyz coordinate axes are referred to as the principal material coordinates, where the x direction is the same as the fiber direction, and the y and z directions are perpendicular to the x direction.
As was explained in the previous sections, SOLID46 with anisotropic material properties has been used to model FRP laminates (Parvin and Granata 2000; Kachlakev et al. 2001; Mahini 2005). Tensiononly membrane SELL41 and elastic SHELL99 have also been used for this purpose (Mirmiran et al. 2000; Hawileh et al. 2012). One possibility to better model FRP in ANSYS which is not tried previously by researchers (although used for modeling reinforcing bars in concrete, (Hunley and Harik 2012)) is to use its reinforced shells and solids elements. These elements constitute a base element that can be reinforced with additional elements. In the case of FRP, the saturant can be used as the base element while fibers are added as reinforcing elements. Figure 6 shows the saturant and the fibers as different element. Reinforcing elements can be defined as discrete or smeared, and they can act as tensiononly, compression only or tension and compression elements. In fact, for FRP, the tensiononly fibers are used. Element SHELL181 can be used as the base element for FRP composite material. Then, it can be reinforced using REINF265 smeared element. Each layer of reinforcement behaves as a unidirectional material. All layers including the base element perform like a parallel system. Perfect bond is assumed amongst the layers. Each layer can have its own thickness (defined as fiber area and space), orientation and local axis coordinate system. This option seems to be most appropriate for modeling FRP sheets in ANSYS. Fibers are embedded inside the base saturant and can have different directions without affecting each other. Even though the fibers are modeled as tensiononly elements, the saturant which represents the base element can be modeled as an elastic element with isotropic properties.
In this study, two options will be considered to model FRP; tensiononly membrane SHELL41 element and membraneonly option of SHELL181 reinforced with REINF265.
Geometry and Meshing
For verification purposes, test subassemblies were modeled in ANSYS taking advantage of plane stress condition of loading. The beam–column subassembly was represented by one row of solid elements. The beam and column sections were scaled down to narrower dimension. Therefore, only one element represents width of the section. Use of one row of solid elements is equivalent to using shell elements with a thickness equal to the width of solid elements. Because ANSYS does not support reinforced concrete shell elements, the solid element is used to represent a condition that would behave similarly to the plane stress case. Width of the solid elements could be chosen arbitrarily. However, in order to have an element aspect ratio close to one, the width is set equal to the mesh size. In this method, the final results are independent of the solid element width. Figure 7 shows the meshed model. All used element types are shown in this figure.
As the beam and column cross section dimension is reduced, the steel rebar and FRP sheets thickness are proportionally reduced. Figure 8 shows how the column and beam cross sections are scaled down. The forces resulted from the analysis have to be scaled up after the analysis as a result, in order to represent forces in the structure. It is worth mentioning that in this kind of scaling, the stresses and deflections in the original and scaled structures remain similar.
Using this method for the finite element analysis considerably reduces the number of elements. Usually in experimental studies, planar loading is applied on specimens. Therefore, the method that is proposed here can be used for any analytical study. Using this method, considerable time is saved, and the designer can use a finer mesh for the planar structure. The attention can thus be shifted from analysing a complex system towards parametric studies on this simpler form and processing of the results.