Using the FEM and considering the environment around the tunnel as an intact rock with elasto-plastic behavior, stresses around a tunnel were studied using the Abaqus Finite Element Analysis (FEA) software [
11]. Because cracks were not explicitly modeled in the numerical model, principal stresses were used as indicators of potential fracturing. Since this solution involves the hydraulics of water flow in the tunnel and the impacts of internal pressures on the surrounding rock, the Hammer software and Abaqus FEA were linked for modeling and analyzing the system. The Hammer software [
12], which works based on the method of characteristics (MOC), was employed to analyze the changes in the internal pressure inside the tunnel, as a function of time. The hydraulic analysis results, from the Hammer software in transient-state conditions, were transferred to the Abaqus FEA in order to analyze stresses in the surrounding rock. It was assumed that, at first, the internal pressure was in the steady-state condition. Afterward, because of sudden gate closure, transient pressures built up in the tunnel. The flowchart below summarizes the main steps in this study (
Figure 1).
2.1. Governing Equations
Using the general Navier–Stokes equation (Equation (1)) and simplifying assumptions—(a) fluid inside the tunnel is non-viscous, (b) fluid velocity fluctuations are ignored, and (c) water has linear compressibility—the hydrodynamic pressure inside the tunnel can be obtained using Equations (1) and (2) [
13].
where
v is the flow velocity (m/s),
μ is the fluid viscosity (Pa·s),
B is the vector of body forces (N),
p is the fluid hydrodynamic pressure in the tunnel (Pa),
K is the bulk modulus (Pa),
t is time (s), and
ρ is the water density (kg/m
3). The only boundary condition governing the fluid inside the tunnel is the boundary between the water and the lining. This boundary condition is defined as in Equation (3) [
13].
where
n is a perpendicular vector to the shared surface between the water and the lining, and
is the second derivative of the lining elements’ displacements in contact with the fluid (m/s
2). The above equation is based on the assumption that the radial displacements of the fluid and lining are similar at the contact surfaces. The connection between the hydrodynamic pressures inside the tunnel {
p} and forces applied to the model caused by the hydrodynamic pressure {
f} are linked by matrix [
Q] (Equation (4)) [
14].
The coupling matrix [
Q] links the hydrodynamic pressures due to gate closure, with forces generated in the concrete lining. This equation is solved by the Abaqus FEA, by applying the boundary and initial conditions. Finally, the displacements and stresses in the rock due to hydrodynamic pressures are calculated. The forces in the concrete lining due to water pressure are transferred to the surrounding rock. As a result, the equilibrium equation in the surrounding rock is as follows [
14]:
where
M,
C, and
K are mass, damping, and hardness matrices, respectively;
Rr is the vector of external forces on the rock;
and
are the second and first derivatives of the rock elements, respectively; and
is the displacement of the rock elements. Equation (6) shows that part of the hydrodynamic force is resisted by the concrete lining (
fs). Therefore, the relationship between hydrodynamic pressure and displacements in the surrounding rock is obtained by linking Equations (4) and (5).
2.2. FEM and Effective Parameters
In the FEM modeling, the following factors were considered in the simulations:
A circular tunnel was excavated in intact rock by a tunnel boring machine (TBM);
Water pore pressure was considered in the concrete lining and in the rock;
The Mohr–Coulomb failure criterion was implemented in order to study stresses in the rock;
A damage plasticity behavior was considered in the concrete lining.
Using a trial-and-error procedure, the model boundaries were selected in a way so as to not affect stress distribution around the tunnel. Therefore, the model boundaries were set at 6d × 25d (d = tunnel diameter) (
Figure 2). More details on the grid and boundary sensitivity analyses are presented in the
Appendix A.
Table 1 shows the mechanical properties of the lining. It was assumed that the tunnel was located above the groundwater level.
The only degree of freedom inside a water pressure tunnel is pressure in the fluid nodes. In Abaqus FEA, acoustic elements possess this feature and are appropriate for simulating the fluid movement inside a tunnel. Since acoustic environments are elastic, shear stresses do not exist in these environments and pressure is proportional to volume strain. In addition, the effects of inertia and compressibility are considered in acoustic elements [
17].
In this study, the interactions between the fluid, lining, and surrounding rock were considered, and the fluid density was set at 1000 kg/m3, with a bulk modulus of 2.07 GPa. Taking into account the interaction between the fluid and lining, the structure surfaces and fluid that are in contact were tied together in Abaqus FEA. Applying the same reasoning, the external nodes of the lining were tied with the nodes of the surrounding rock due to structure–rock interactions.
The environment around the tunnel has in situ stresses. By defining the height, specific weight, and the lateral stress coefficients of the rock, equilibrium conditions between the horizontal and vertical stresses were achieved, which resulted in zero ground settlement before tunnel excavation.
Since the transient pressure inside the tunnel depends on factors such as gate operations, this pressure was applied to the model as a quasi-static load (by gradually increasing the loading, so that the impacts of inertia became negligible). This means that, at different times, different pressures were applied to the lining. In order to apply the time-variable pressure to all of the nodes in the acoustic environment, the amplitude function in Abaqus FEA was used.
The plane strain elements with linear interpolation function were employed to mesh the surrounding rock and concrete lining. In Abaqus FEA, these types of elements are called CPE4R (continuum plain strain element 4-node reduced integration). Meshing was such that, by approaching the tunnel section, the mesh size decreased to achieve more precise results. Moreover, plane stress family elements were used for meshing the lining. In Abaqus FEA, these elements are called CPS4R (continuum plain stress element 4-node reduced integration). Furthermore, in the lining and rock elements, the reduced integration method was implemented, and AC2D4 elements (acoustic continuum 2-dimension 4-node) were used to simulate water transient pressure inside the tunnel [
11,
18].
The first step in this research study was simulating in situ stresses. In order to have zero ground-surface settlement before tunnel excavation, these stresses should satisfy Equations (7) and (8) [
19].
where
γr is the specific weight of the rock,
h is the height of the overburden rock, and
k0 is the coefficient of lateral rock pressure. In the next step, the tunnel excavation was simulated. It was assumed that the tunnel was excavated by a tunnel boring machine. At this stage, the release of stress and displacements occurred in the rock. After the tunnel cross-section, the concrete lining was simulated. In this step, a concrete lining with the specifications presented in
Table 1 was modeled. Interaction between the rock and the lining was considered using tangential and normal stiffnesses. The final step was applying steady-state conditions and hydrodynamic water pressure to the lining. It was assumed that the transient pressure inside the tunnel would occur due to the turbine gate closure in a typical hydropower plant (
Figure 3).
Using the Hammer software, hydraulic analyses were performed in steady-state and transient-state conditions, by defining the characteristics of the duct (water tunnel), reservoir, and gate closure schedule. The parameters used for these analyses and their values are presented in
Table 2 and
Table 3. Water velocity was considered to be 6 m/s, according to the recommended value by the United States Bureau of Reclamation [
20]. Moreover, in order to create critical conditions in the tunnel to determine its bearing capacity, it was assumed that the surge tank was disabled. The maximum flow rate was considered to be 60 m
3/s, and, according to the gate closure time in typical water tunnels, the gate closure times were considered to be 14 s (fast), 18 s (normal), and 26 s (slow). Furthermore, based on the duct characteristics, the pressure wave velocity according to the characteristics of the duct was determined by Equation (9), where
D is the inner diameter of the tunnel,
E is the elastic concrete modulus, and
tc is the lining thickness [
21].
It was assumed that the lining could expand in the longitudinal direction, which results in a λ (confinement coefficient) value of 1 [
21].
The location for investigating stresses in the rock was considered to be near the penstock (Node C) in the tunnel path. Finally, the pressure values at this point, obtained by the Hammer software, were input to the Abaqus FEA, under hydrodynamic pressure loadings.
2.3. Parametric Study in Steady-State Conditions
In this study, the bearing capacity of the pressure tunnel under a steady-state condition was investigated. The bearing capacity of a concrete-lined pressure tunnel is dependent either on the tensile strength of the surrounding rock only, or both the concrete and the rock. Generally, in pressure tunnels that are excavated in intact rock, the concrete lining does not contribute to the stability of the tunnel during excavation and only provides an appropriate bed for water to be conveyed toward the turbine.
Crack formation in the surrounding rock (hydraulic fracturing), due to high internal pressure, shows that the pressure tunnel reached its ultimate capacity; therefore, a parametric study was performed to investigate the impact of overburden height on the ultimate bearing capacity of the pressure tunnel in a steady-state condition.
Figure 4 shows the effective parameters in the bearing capacity of a tunnel.
Pe(
pi) is the water pressure on the outer surface of the concrete lining due to seepage. According to Equation (10), this parameter is dependent on internal pressure, and it was calculated using the FEM in the present study [
22].
where
t (thickness of the lining),
k0,
kr (hydraulic conductivity of the rock), and
γr (specific weight of the rock) were considered constant for all analyses, and their values are presented in
Table 4. Moreover, the values for
Er,
C,
φ, and
h are presented in
Table 5.
In each analysis, the bearing capacity of the tunnel was determined by increasing the internal pressure (pi) to the point at which the first crack was formed in the surrounding rock. In this situation, the corresponding pi was considered as the failure threshold, which indicates the ultimate bearing capacity of the tunnel.