Products: ABAQUS/Standard ABAQUS/Explicit
ABAQUS provides constitutive models suitable for brittle materials such as concrete in which cracking is important. These models are intended for unreinforced as well as reinforced concrete structures. The problem described here illustrates the use of the concrete damaged plasticity model, which is available in both ABAQUS/Standard and ABAQUS/Explicit, for the analysis of an unreinforced notched concrete beam under 3-point bending. This problem is chosen because it has been studied extensively both experimentally by Petersson (1981) and analytically by Rots et al. (1984, 1985), de Borst (1986), and Meyer et al. (1994), among others. The predominant behavior is Mode I cracking, so the example provides good verification of this aspect of the constitutive model. We also have the advantage that this beam experiment has been repeated by a number of different researchers, and there is good material information about important parameters, such as the Mode I fracture energy, 
. Thus, we can directly compare the numerical results with the experimental results with minimal uncertainty. We also investigate the sensitivity of the numerical results to the finite element discretization and to the choice of cracking material properties.
The concrete damaged plasticity model in ABAQUS provides a general capability for modeling plain or reinforced concrete in the applications of monotonic, cyclic, and/or dynamic loading. This model can be used to simulate the irreversible damage involved in the fracturing process and the recovery of stiffness as loads change from tension to compression or vice versa. In addition, this model can include strain rate dependency. For more details on this model, see “Concrete damaged plasticity,” Section 18.5.3 of the ABAQUS Analysis User's Manual.
In addition to the concrete damaged plasticity model, ABAQUS provides the smeared cracking concrete model in ABAQUS/Standard and the brittle cracking model in ABAQUS/Explicit. For a description of these models, see “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 notched beam is shown in Figure 3.2.11–1. Because of symmetry, only one half of the beam is modeled. Figure 3.2.11–2 shows the three meshes used for this problem: a coarse mesh of 70 elements, a medium mesh of 280 elements, and a fine mesh of 1120 elements. We model the beam using plane stress (CPS4R) elements and three-dimensional (C3D8R) elements to provide verification of both element types.
The beam has a Young's modulus of 30 GPa (4.35 × 106 lb/in2), a Poisson's ratio of 0.20, a density of 2400 kg/m3 (0.225 × 10–3 lb s2/in4), a cracking failure stress of 3.33 MPa (482.96 lb/in2), and a Mode I fracture energy of 124 N/m (0.708 lb/in). The fracture energy value, , defines the area under the postcracking stress-displacement curve. The effect of different postcracking softening behavior is the subject of one of the studies carried out in this example.
The beam is loaded by prescribing the vertical displacement at the center of the beam until it reaches a value of 0.0015 m.
The Riks method is used in ABAQUS/Standard since the behavior of the beam is quite unstable when cracking progresses.
ABAQUS/Explicit is a dynamic analysis program. In this case we are interested in static solutions; hence, care must be taken that the beam is loaded slowly enough to eliminate significant inertia effects. For problems involving brittle failure, this is especially important since the sudden drops in load carrying capacity that normally accompany brittle behavior generally lead to increases in the kinetic energy content of the response. Therefore, the beam is loaded by applying a velocity that increases linearly from 0 to 0.06 m/s over a period of 0.05 seconds to obtain the final displacement of 0.0015 m at the center of the beam. This ensures a quasi-static solution (the kinetic energy in the beam is small throughout the response) in a reasonable number of time increments. Nevertheless, oscillations in the load-displacement response caused by inertia effects are still visible, mainly after the concrete has cracked significantly.
The speed of application of the loading in ABAQUS/Explicit is the subject of another study in this problem.
Results are described below for each analysis variation.
The three finite element meshes described earlier are used to show the influence of mesh refinement on the load-displacement response of the concrete beam.
Since there is no reinforcement in this problem, the postfailure behavior is specified in terms of the stress-displacement response (*TENSION STIFFENING, TYPE=DISPLACEMENT) to minimize mesh sensitivity. We can also specify the postfailure behavior directly in terms of the fracture energy, (*TENSION STIFFENING, TYPE=GFI). The fracture energy method assumes a linear loss of strength after cracking. Thus, if we specify the tension softening behavior in terms of stress versus cracking displacement and assume a linear curve (
, 0), (0, 
/
) as shown in Figure 3.2.11–3, the above two methods will give the same results. Tensile damage is specified in terms of the tension damage variable, 
, versus the cracking displacement (*CONCRETE TENSION DAMAGE, TYPE=DISPLACEMENT). A linear dependence—(0, 0), (0.9, 
)—is assumed for this study, as shown in Figure 3.2.11–4. For the constitutive calculations, ABAQUS automatically converts the cracking displacement values to “plastic” displacement values using the relationship
, is assumed to be one unit; (i.e., 
). Care must be taken in specifying the tension damage to ensure that the calculated plastic strain (or displacement) is positive and monotonically increasing with increasing cracking strain (or displacement).The load-displacement response of the notched beam obtained for the three meshes with ABAQUS/Standard is shown in Figure 3.2.11–5 for the three-dimensional models and in Figure 3.2.11–6 for the plane stress models. The load-displacement response obtained with ABAQUS/Explicit is shown in Figure 3.2.11–7 for the three-dimensional models and in Figure 3.2.11–8 for the plane stress models. These figures show that the three-dimensional and plane stress models in ABAQUS/Standard are in close agreement. Minor differences are observed in the results obtained with ABAQUS/Explicit; these can be attributed primarily to dynamic effects. Three-dimensional models have a relatively higher level of mesh sensitivity due to the effect of possible cracking in the out-of-plane direction. For the two-dimensional models, although a small amount of mesh sensitivity remains between the coarse mesh and the other two meshes, the medium and fine meshes give similar results. Based on these observations, all subsequent studies are done using the plane stress medium mesh. All the curves shown are smoothed. Displaced shapes obtained with ABAQUS/Standard for the three plane stress meshes are shown in Figure 3.2.11–9. The three-dimensional meshes and the ABAQUS/Explicit meshes show essentially the same deformation. The expected Mode I fracture pattern is observed consistently in all meshes.
The results described above are obtained using linear tension softening. Such a choice of softening leads to a response that is too stiff compared with the experimental observations of Petersson. In this study we use three different evolutions of the stress as a function of the cracking displacement. We compare the linear variation used previously to two tension softening functions where the cracking stress is reduced more rapidly as the crack initiates. These functions are shown in Figure 3.2.11–10: one consists of a two-segment representation of softening, and the other is a four-segment representation. The area under the softening curve is the same in all cases so that the value of the Mode I fracture energy of the material is preserved. Different linear tension damage curves are used for each tension softening model in this study to ensure that the plastic displacement is positive and monotonically increasing with increasing cracking displacement for all three tension softening curves.
The load-displacement responses obtained with ABAQUS/Standard for the three tension softening representations are shown in Figure 3.2.11–11 for the plane stress medium mesh. For ABAQUS/Explicit the responses are shown in Figure 3.2.11–12 for the plane stress medium mesh. It is clear that more rapid reductions of the cracking stress after initial cracking lead to less stiff responses. The modeling of tension softening is a key determinant of the peak/failure response. The two-segment and four-segment softening models provide peak/failure responses that agree well with the experimental observations of Petersson. The initial linear responses of the calculated results are slightly softer than the experimental results. This small difference is because a relatively blunt notch is used in this study, while a much sharper cast notch was used in Petersson (1981). All the curves shown have been smoothed.
The quasi-static solutions obtained in the previous ABAQUS/Explicit studies still show some oscillations due to inertia effects, albeit somewhat hidden by the fact that curve smoothing is used. This additional exercise is intended to show the difference between the unsmoothed and smoothed responses obtained at the loading speed used thus far (0.06 m/s) and an analysis where the loading is applied at a much lower speed (0.005 m/s).
Figure 3.2.11–13 shows the results obtained for the plane stress medium mesh with four-segment tension softening. Smoothing of the faster load-displacement response (19635 analysis increments) is shown to match reasonably well the load-displacement response obtained at the slower speed (235830 analysis increments). Since the slower response does not provide much more useful information, we conclude that we are justified to run at the faster speed and to use smoothing to present the quasi-static response.
Coarse mesh response.
Medium mesh response.
Fine mesh response.
Coarse mesh response.
Medium mesh response.
Fine mesh response.
Medium mesh response with *TENSION STIFFENING, TYPE=GFI.
Medium mesh, one-segment tension softening response with *TENSION STIFFENING, TYPE=DISPLACEMENT.
Medium mesh, two-segment tension softening response with *TENSION STIFFENING, TYPE=DISPLACEMENT.
Medium mesh, four-segment tension softening response with *TENSION STIFFENING, TYPE=DISPLACEMENT.
Coarse mesh response.
Medium mesh response.
Fine mesh response.
Coarse mesh response.
Medium mesh response.
Fine mesh response.
Medium mesh, one-segment tension softening response.
Medium mesh, two-segment tension softening response.
Medium mesh, four-segment tension softening response.
Medium mesh, 0.005 m/s speed response.
de Borst, R., Ph. D. thesis, Delft University of Technology, The Netherlands, 1986.
Meyer, R., H. Ahrens, and H. Duddeck, “Material Model for Concrete in Cracked and Uncracked States,” Journal of Engineering Mechanics Division, ASCE, vol. 120, EM9, pp. 1877–1895, 1994.
Petersson, P. E., “Crack Growth and Development of Fracture Zones in Plain Concrete and Similar Materials,” Report No. TVBM-1006, Division of Building Materials, University of Lund, Sweden, 1981.
Rots, J. G., G. M. A. Kusters, and J. Blaauwendraad, “The Need for Fracture Mechanics Options in Finite Element Models for Concrete Structures,” Computer-Aided Analysis and Design of Concrete Structures, Pineridge Press, Swansea, United Kingdom, pp. 19–32, 1984.
Rots, J. G., P. Nauta, G. M. A. Kusters, and J. Blaauwendraad, “Smeared Crack Approach and Fracture Localization in Concrete,” HERON, Delft University of Technology, The Netherlands, vol. 30, no.1, 1985.
