Symmetry conditions allow us to model one-quarter of the slab. A 3 × 3 mesh of 8-node shell elements is used for the ABAQUS/Standard analysis. No mesh convergence studies have been performed, but the reasonable agreement between the analysis results and the experimental data suggests that the mesh is adequate to predict overall response parameters with usable accuracy. Three different meshes are used in ABAQUS/Explicit to assess the sensitivity of the results to mesh refinement: a coarse 6 × 6 mesh, a medium 12 × 12 mesh, and a fine 24 × 24 mesh of S4R elements. Nine integration points are used through the thickness of the concrete to ensure that the development of plasticity and failure is modeled adequately. The two-way reinforcement is modeled using the *REBAR LAYER option. Symmetry boundary conditions are applied on the two edges of the mesh, and the corner point is restrained in the transverse direction.

The material data are given in Table 1.1.5–1. The material properties of concrete are taken from Gilbert and Warner (1978). Some of these data are assumed values, because they are not available for the concrete used in the experiment. The assumed values are taken from typical concrete data. The compressive behavior of concrete in the cracking model in ABAQUS/Explicit is assumed to be linear elastic. This is a reasonable assumption for a case such as this problem, where the behavior of the structure is dominated by cracking resulting from tension in the slab under bending.

The modeling of the concrete-reinforcement interaction and the energy release at cracking is of critical importance to the response of a structure such as this once the concrete starts to crack. These effects are modeled in an indirect way by adding “tension stiffening” to the plain concrete model. This approach is described in “A cracking model for concrete and other brittle materials,” Section 4.5.3 of the ABAQUS Theory Manual; “Concrete smeared cracking,” Section 18.5.1 of the ABAQUS Analysis User's Manual; and “Cracking model for concrete,” Section 18.5.2 of the ABAQUS Analysis User's Manual. The simplest tension stiffening model defines a linear loss of strength beyond the cracking failure of the concrete. In this example three different values for the strain beyond failure at which all strength is lost (5 × 10^–4, 1 × 10^–3, and 2 × 10^–3) are used to illustrate the effect of the tension stiffening parameters on the response.

Since the response is dominated by bending, it is controlled by the material behavior normal to the crack planes. The material's shear behavior in the plane of the cracks is not important. Consequently, the choice of shear retention has no significant influence on the results. In ABAQUS/Explicit the shear retention chosen is exhausted at the same value of the crack opening at which tension stiffening is exhausted. In ABAQUS/Standard full shear retention is used because it provides a more efficient numerical solution.

Since considerable nonlinearity is expected in the response, including the possibility of unstable regimes as the concrete cracks, the modified Riks method is used with automatic incrementation in the ABAQUS/Standard analysis. With the Riks method the load data and solution parameters serve only to give an estimate of the initial increment of load. In this case it seems reasonable to apply an initial load of 1112 N (250 lb) to the quarter-model for a total initial load on the structure of 4448 N (1000 lb). This can be accomplished by specifying a load of 22241 N (5000 lb) and an initial time increment of 0.05 out of a total time period of 1.0. The analysis is terminated when the central displacement reaches 25.4 mm (1 in).

Since ABAQUS/Explicit is a dynamic analysis program and in this case we are interested in static solutions, the slab must be loaded slowly enough to eliminate any significant inertia effects. The slab is loaded in its center by applying a velocity that increases linearly from 0 to 2.0 in/second such that the center displaces a total of 1 inches in 1 second. This very slow loading rate ensures quasi-static solutions; however, it is computationally expensive. The CPU time required for this analysis can be reduced in one of two ways: the loading rate can be increased incrementally until it is judged that any further increase in loading rate would no longer result in a quasi-static solution, or mass scaling can be used (see “Explicit dynamic analysis,” Section 6.3.3 of the ABAQUS Analysis User's Manual). These two approaches are equivalent. Mass scaling is used here to demonstrate the validity of such an approach when it is used in conjunction with the brittle cracking model. Mass scaling is done by increasing the density of the concrete and the reinforcement by a factor of 100, thereby increasing the stable time increment for the analysis by a factor of 10 and reducing the computation time by the same amount while using the original slow loading rate. Figure 1.1.5–4 shows the load-deflection response of the slab for analyses using the 12 × 12 mesh with and without mass scaling. The mass scaling used does not affect the results significantly; therefore, all subsequent analyses are performed using mass scaling.