2.1.15 Seismic analysis of a concrete gravity dam
Products: Abaqus/Standard Abaqus/Explicit
In this example we consider an analysis of the Koyna dam, which was subjected to an earthquake of magnitude 6.5 on the Richter scale on December 11, 1967. The example illustrates a typical application of the concrete damaged plasticity material model for the assessment of the structural stability and damage of concrete structures subjected to arbitrary loading. This problem is chosen because it has been extensively analyzed by a number of investigators, including Chopra and Chakrabarti (1973), Bhattacharjee and Léger (1993), Ghrib and Tinawi (1995), Cervera et al. (1996), and Lee and Fenves (1998).
Problem description
The geometry of a typical non-overflow monolith of the Koyna dam is illustrated in Figure 2.1.15–1. The monolith is 103 m high and 71 m wide at its base. The upstream wall of the monolith is assumed to be straight and vertical, which is slightly different from the real configuration. The depth of the reservoir at the time of the earthquake is = 91.75 m. Following the work of other investigators, we consider a two-dimensional analysis of the non-overflow monolith assuming plane stress conditions. The finite element mesh used for the analysis is shown in Figure 2.1.15–2. It consists of 760 first-order, reduced-integration, plane stress elements (CPS4R). Nodal definitions are referred to a global rectangular coordinate system centered at the lower left corner of the dam, with the vertical y-axis pointing in the upward direction and the horizontal x-axis pointing in the downstream direction. The transverse and vertical components of the ground accelerations recorded during the Koyna earthquake are shown in Figure 2.1.15–3 (units of g = 9.81 m sec–2). Prior to the earthquake excitation, the dam is subjected to gravity loading due to its self-weight and to the hydrostatic pressure of the reservoir on the upstream wall.
For the purpose of this example we neglect the dam–foundation interactions by assuming that the foundation is rigid. The dam–reservoir dynamic interactions resulting from the transverse component of ground motion can be modeled in a simple form using the Westergaard added mass technique. According to Westergaard (1933), the hydrodynamic pressures that the water exerts on the dam during an earthquake are the same as if a certain body of water moves back and forth with the dam while the remainder of the reservoir is left inactive. The added mass per unit area of the upstream wall is given in approximate form by the expression
,
with , where = 1000 kg/m3 is the density of water. In the Abaqus/Standard analysis the added mass approach is implemented using a simple 2-node user element that has been coded in user subroutine UEL. In the Abaqus/Explicit analysis the dynamic interactions between the dam and the reservoir are ignored.
The hydrodynamic pressures resulting from the vertical component of ground motion are assumed to be small and are neglected in all the simulations. Material properties
The mechanical behavior of the concrete material is modeled using the concrete damaged plasticity constitutive model described in “Concrete damaged plasticity,” Section 23.6.3 of the Abaqus Analysis User's Manual, and “Damaged plasticity model for concrete and other quasi-brittle materials,” Section 4.5.2 of the Abaqus Theory Manual. The material properties used for the simulations are given in Table 2.1.15–1 and Figure 2.1.15–4. These properties are assumed to be representative of the concrete material in the Koyna dam and are based on the properties used by previous investigators. In obtaining some of these material properties, a number of assumptions are made. Of particular interest is the calibration of the concrete tensile behavior. The tensile strength is estimated to be 10% of the ultimate compressive strength ( = 24.1 MPa), multiplied by a dynamic amplification factor of 1.2 to account for rate effects; thus, = 2.9 MPa. To avoid unreasonable mesh-sensitive results due to the lack of reinforcement in the structure, the tensile postfailure behavior is given in terms of a fracture energy cracking criterion by specifying a stress/displacement curve instead of a stress-strain curve, as shown in Figure 2.1.15–4(a). This is accomplished with the postcracking stress/displacement curve. Similarly, tensile damage, , is specified in tabular form as a function of cracking displacement by using the postcracking damage displacement curve. This curve is shown in Figure 2.1.15–4(b). The stiffness degradation damage caused by compressive failure (crushing) of the concrete, , is assumed to be zero. Damping
It is generally accepted that dams have damping ratios of about 2–5%. In this example we tune the material damping properties to provide approximately 3% fraction of critical damping for the first mode of vibration of the dam. Assuming Rayleigh stiffness proportional damping, the factor required to provide a fraction as
of critical damping for the first mode is given
. From a natural frequency extraction analysis of the dam the first
= 18.61 rad sec–1 (see Table 2.1.15–2). Based on this, is
eigenfrequency is found to be chosen to be 3.23 × 10–3 sec. Loading and solution control
Loading conditions and solution controls are discussed for each analysis. Abaqus/Standard analysis
Prior to the dynamic simulation of the earthquake, the dam is subjected to gravity loading and hydrostatic pressure. In the Abaqus/Standard analysis these loads are specified in two consecutive static steps, using a distributed load with the load type labels GRAV (for the gravity load) in the first step and HP (for the hydrostatic pressure) in the second step. For the dynamic analysis in the third step the transverse and vertical components of the ground accelerations shown in Figure 2.1.15–3 are applied to all nodes at the base of the dam.
Since considerable nonlinearity is expected in the response, including the possibility of unstable regimes as the concrete cracks, the overall convergence of the solution in the Abaqus/Standard analysis is expected to be non-monotonic. In such cases automatically setting the time incrementation parameters is generally recommended to prevent premature termination of the equilibrium iteration process because the solution may appear to be diverging. The unsymmetric matrix storage and solution scheme is activated by specifying an unsymmetric equation solver for the step. This is essential for obtaining an acceptable rate of convergence with the concrete damaged plasticity model since plastic flow is nonassociated. Automatic time incrementation is
used for the dynamic analysis of the earthquake, with the half-increment residual tolerance set to 107 and a maximum time increment of 0.02 sec. Abaqus/Explicit analysis
While it is possible to perform the analysis of the pre-seismic state in Abaqus/Explicit, Abaqus/Standard is much more efficient at solving quasi-static analyses. Therefore, we apply the gravity and hydrostatic loads in an Abaqus/Standard analysis. These results are then imported into Abaqus/Explicit to continue with the seismic analysis of the dam subjected to the earthquake accelerogram. We still need to continue to apply the gravity and hydrostatic pressure loads during the explicit dynamic step. In Abaqus/Explicit gravity loading is specified in exactly the same way as in Abaqus/Standard. The specification of the hydrostatic pressure, however, requires some extra consideration because this load type is not currently supported by Abaqus/Explicit. Here we apply the hydrostatic pressure using user subroutine VDLOAD.
The Abaqus/Explicit simulation requires a very large number of increments since the stable time increment (6 × 10–6 sec) is much smaller than the total duration of the earthquake (10 sec). The analysis is run in double precision to prevent the accumulation of round-off errors. The stability limit could be increased by using mass scaling; however, this may affect the dynamic response of the structure.
For this particular problem Abaqus/Standard is computationally more effective than Abaqus/Explicit because the earthquake is a relatively long event that requires a very large number of increments in Abaqus/Explicit. In addition, the size of the finite element model is small, and the cost of each solution of the global equilibrium equations in Abaqus/Standard is quite inexpensive.
Results and discussion
The results for each analysis are discussed in the following sections. Abaqus/Standard results
The results from a frequency extraction analysis of the dam without the reservoir are summarized in Table 2.1.15–2. The first four natural frequencies of the finite element model are in good agreement with the values reported by Chopra and Chakrabarti (1973). As discussed above, the frequency extraction analysis is useful for the calibration of the material damping to be used during the dynamic simulation of the earthquake.
Figure 2.1.15–5 shows the horizontal displacement at the left corner of the crest of the dam relative to the ground motion. In this figure positive values represent displacement in the downstream direction. The crest displacement remains less than 30 mm during the first 4 seconds of the earthquake. After 4 seconds, the amplitude of the oscillations of the crest increases substantially. As discussed below, severe damage to the structure develops during these oscillations.
The concrete material remains elastic with no damage at the end of the second step, after the dam has been subjected to the gravity and hydrostatic pressure loads. Damage to the dam initiates during the seismic analysis in the third step. The evolution of damage in the concrete dam at six different times during the earthquake is illustrated in Figure 2.1.15–6, Figure 2.1.15–7, and Figure 2.1.15–8. Times = 3.96 sec, = 4.315 sec, and = 4.687 sec correspond to the first three large excursions of the crest in the upstream direction, as shown in Figure 2.1.15–5. Times = 4.163 sec and = 4.526 sec correspond to the first two large excursions of the crest in the downstream direction. Time = 10 sec corresponds to the end of the earthquake. The figures