Finite Element Modelling and Simulation of Tunnel Gates of Dam Structures in ABAQUS Using Reduced-Integrated 8-Node Hexahedral Solid-Shell Element

,


Introduction
The safety of dams depends largely on the safety of their gates.The number of dams with gates for the efficient use of water is increasing.More than a third of all large dams have gates, and most of these are flood control dams that regulate floods and other water discharges.The invention and earlier use of gates date to 1490 [1].The most common types of vertical lift gates used for hydraulic structures are stone gates, tracked gates, gates with fixed wheels, and sliding gates.Vertical lift gates with wheels on the sides to reduce friction are called fixed wheel gates, while gates without wheels are called sliding gates.A radial gate differs from a flat gate, an arm gate, which is used in both dams and canal locks to control the flow of water.A method for developing an optimal design of radial gates using steel sections and different types of steel was investigated [2].
The gates are mainly used for operational, emergency, and maintenance purposes in dams or irrigation canals.An optimal design of the lifting mechanism and a wellequipped and efficient control system for lifting the gate are also important.The two-dimensional dam failure analysis of Berdan Dam for floodplains and the preparation of emergency plans using GIS data are presented by Unal [3].It is also important to control the water in the tunnel gates of dams in case of flooding.If the gate fails or does not open at the required speed, this poses a major problem for the dam [4] and ultimately for public safety.
The standards and regulations for dam construction do not address the connection between the gate and the main reinforced concrete structure [5][6][7].Only the standards require a 3D analysis and design for the tunnel and diversion structures in Section 2.2 of reference [5].The design analysis of water protection sliding gates for diversion dams is investigated using CFD and ANSYS [8,9].The novelty of this research work is that there is no published work on 3D finite element modelling and simulation of tunnel gate structures including their connections and construction phases, which are very important and critical parts of dams exposed to the maximum water level in the reservoir.A case study with real details of the construction project for nonlinear finite element modelling and simulation of the diversion tunnel gate of Gokdere Bridge Dam in Adana, Turkey, is presented.
On the other hand, there are many studies on concrete damage models, experimental and numerical solutions, and failure and seismic analysis of dams for dam safety.By combining experiments and numerical solutions, the damage characteristics of the dam body under the action of various water explosions are investigated for a 50-meter-high gravity concrete dam [10].A damage analysis for arch concrete dams with underwater explosion loading is carried out [11].A plastic damage model for the cyclic loading of the concrete was developed by Lee and Fenves [12] for the seismic analysis of the concrete dams.Mesoscale 3D fracture modelling and validation of the concrete based on in situ X-ray computed tomography images using a damage plasticity model [13] with damage and fracture profiles and for damage calculations [14] with Monte Carlo simulations of the dynamic compressive behavior of the concrete are investigated.In the mesomodels, the damage usually starts around the largest voids.gates (four wings) of the diversion tunnel are sliding gates with guide rollers (see Figure 3).Rubber seals on the four downstream sides ensure water tightness.The gates are moved by a mobile crane.The first gate, the second gate, and the other gate wings are lowered, and the water in the diversion tunnel is stopped when the gate is closed (see Figure 1).Below you will find the project drawings and reinforced concrete details of the gate structure of the diversion tunnel.The sections and the front part of the reinforced concrete gate structure of the diversion tunnel are shown in Figure 4 with dimensions and elevations.Figures 5-7 show the concrete of the first and second phases and the details of the steel anchor connections used in the construction.In the figures, the gray part is the first phase of the concrete structure and the shaded part is the second phase of the concrete structure.
In the construction project, the anchors and their plates remain in the first phase of the concrete (the gray part in Figure 7).Before the concrete of the second phase is placed, the remaining anchors are mounted on slabs and steel sections.In order to transfer the load of the gates to the concrete of the first and second phases and the load of the gates to the bond with the steel plates and the anchors, the welding of the buried plates should be done by the technique and the load should be transferred, the buried

Second phase concrete
First phase concrete  The condition of the upper and lower flanges of the steel I-profile into which the gate is pressed is as follows: upper flange: one piece, 22 mm thick, and 400 mm wide and lower flange: 22 mm thick and 250 mm wide.In addition, the head of the flake lying in the direction of flow is 100 mm.The weld seam thickness of the lower flange of the I-profile is 10 mm.The weld seam of the upper and lower flanges of the I-profile is 7 mm.These welds are circumferential (Figure 8).The anchors, which determine the behavior of the composite system with the concrete and steel elements of the 2nd phase, are important for the anchors.
There is a steel plate on the underside of the beam that ensures tightness and to which the steel plate should be attached.The thickness of the beam is 250 mm, as shown in Figure 9.The anchorage lengths and types in phase 1 and phase 2 of the concrete are shown in Figure 10.

Linear and Nonlinear Finite Element Modelling of Tunnel Gates of Dam Structure
A model containing all elements (steel plate and section, anchors, and concrete) and nonlinear elastic properties of the materials is created to see the real behavior of the composite structure for the 3D finite element model of the gate structure.The concrete thicknesses, number of anchors and dimensions, steel plate, and profile dimensions are also considered in a detailed project.Nonlinear analyses were performed to show the actual behavior and strength of the structure.
For the linear and nonlinear finite element modelling in ABAQUS [15], the gate structure is considered in the 3dimensional finite element model, as shown in Figures 1  and 2, considering the details of the design project.This is important for the behavior of the composite structure.The analyses performed in the ABAQUS model were also performed using the nonlinear analysis method.The hydrostatic loads from the gate were transferred through steel plates, sections, and anchors with composite material and nonlinear behavior.
The structure of the tunnel gate consists of two-phase concrete and is supported by I-beams and anchors.This structural model is analyzed using the 3D finite element method.For this purpose, the universal finite element program ABAQUS is used for the modelling of the concrete and steel elements.The 3D C3D8R hexahedral solid elements shown in Figure 11 are used.To model the system realistically, the dimensions of the elements are set to approximately 5 cm.Each finite element has 8 nodes, an isoparametric property, and a reduced integration capacity.In nonlinear analysis, the terms "Concrete damaged plasticity", "Concrete tension stiffening", "Concrete tension damage", and "Concrete compression damage" are used.
For the behavior of contact surfaces, "SURFACE INTERACTION" with the option "GAP" or "INTERFACE" is specified in the ABAQUS Keywords Reference Manual [16]: "CONTACT CONTROLS", "GAP", "INTERFACE", AND "SURFACE INTERACTION".Friction behavior for surface-based contact, when the surfaces are in contact, normally transmits both shear and normal forces across their interface with the "SURFACE INTERACTION" and "FRIC-TION" command.The active D.O.F. 1, 2, 3, 4, 5, and 6 were used for the connecting element.The steel profile is subject to the same degree of freedom at all contact points for load transfer and the bond between anchor elements and concrete.
Explicit modelling of the interface between steel and concrete is of greater importance for the interaction of composite materials.Hai et al. [17] explicitly simulate the bonding and debonding behavior at the interface for mesoscale failure mechanisms of ultrahigh strength fiber-reinforced concrete.Another approach is to explicitly model the        11 Modelling and Simulation in Engineering bond-slip behavior at the interface by inserting a cohesive interface element with a thickness of zero [18].
The dimensions of the concrete used for the modelling are shown in Figure 12.The dimensions of the steel sections, plates, and anchors are shown in Figure 13 for a 2 m long component.The 3D finite element modelling of the steel plates and anchors is shown in Figure 14.
The area under which the gate load is applied is the concrete mass.It is limited to a volume of 1165 mm * 1500 mm * 2000 mm.The part cut out for the finite element  12 Modelling and Simulation in Engineering     When calculating the pressure area of the gate, the pressure area on the upper side was calculated as 7 75 × 0 125 = 0 96875 m 2 .The total discharge area of the gate is 5.78125 m 2 .9 625 × 0 5 = 4 8125 m 2 of this area must be the lateral pressure area.When calculating the area on which the load is transferred from the gates to the support, as shown in Figure 15, the load is not transferred from the gate to the upper support surface, as this section is only closed with a seal (Figure 20) and does not serve as a complete support.For this reason, this section was not included in the calculations (to be on the safe side).
The points at which the gate exerts pressure on the side supports are shown in Figures 15 and 19.If both side supports are considered, the total area to which the gate loads are transferred to the side supports is 9 625 × 0 40 × 2 = 7 70 m 2 .Figure 21 shows that the load distribution is composed due to the I-shaped steel profile in the lateral supports that contains the bolts and anchors in the concrete.The load is transferred from the gate to the supports: the compressive force on the supports is simply calculated as follows: P = 85 00 × 7 75 × 10 00 = 6587 50 tons (the height of the water is 85 meters).Taking into account the hydrostatic pressure on the concrete in the support area, the support area to which the load is transferred (considering the load on the gate) is as follows: The quality of the concrete was specified as C25 (25 MPa, 2500 t/m 2 ).According to TS500/2000 [19] Article 6.2.5, the coefficient of the concrete material in the case of the collapse analysis of the existing structure is assumed to be 1.0.If this coefficient is 1.0, the concrete compressive stress to be used for the calculation is 2500 t/m 2 .The calculated concrete compressive stress (855.52 t/m 2 ) is less than 2500 t/m 2 , so no concrete crush will occur.
The concrete compressive stresses determined above were calculated using simple methods and do not exceed the limit values.The real load distribution and the stresses are analyzed using the 3D finite element method and the ABAQUS program.The maximum concrete compressive stress determined in these analyses is below the value for the maximum compressive stress, and there is no crushing of the concrete as in the results of the nonlinear analysis of ABAQUS.

Linear and Nonlinear Simulations for
Cracking and Collapse of Structure 4.1.Linear Analysis of the Gate Structure.The maximum and minimum pressures, tensile stresses, and unit deformations are shown in Figure 22.The maximum compressive deformation is 4 6 × 10 −6 .The maximum permissible compressive deformation of this concrete is 3 5 × 10 −3 .The unit deformation between the concrete of the first and second phases is between 1 8 × 10 −4 and 9 4 × 10 −5 (Figure 22).The maximum compressive stress is 13.31 MPa, and the compressive stress between the first and second phases is between 5 and 8 MPa (Figure 23).The maximum displacement due to the applied pressure is 0.2 mm, as you can see in Figure 24.
The maximum tensile deformation per unit is 2 63 × 10 −4 (Figure 25).This shows that the concrete has exceeded the linear limit.Therefore, the nonlinear analysis was preferred for the capacity analysis.The maximum tensile stress in concrete is between 6.63 and 8.29 MPa.The maximum tensile stress in steel structures is 76 MPa.The tensile stress between the concrete of the first and second phases is between 1 5 × 10 −5 and 1.66 MPa (see Figure 26).

Nonlinear Analysis of Gate
Structure.The results of the nonlinear analysis are shown below.For the nonlinear analysis, the material properties given in Figure 17 for concrete and in Figure 18 for steel are used.The "Concrete Damage Model/Concrete Damage Plasticity Model" and the "Tension Stiffening" model in ABAQUS are considered.
In the nonlinear analysis, the maximum compressive stress of the concrete is given as 13.4 MPa (Figure 27).This value is lower than 25 MPa, the maximum strength of the concrete.The maximum stresses of the steel in the nonlinear analysis are 108 MPa (Figure 28).The deformations in the nonlinear analysis of the gate structure are shown in Figure 29.

Simulations for Nonlinear Capacity Analysis of Gate
Structure.Simulations for the nonlinear analysis have shown that the system does not collapse at a water height of 85 meters.To see whether the system collapses or not, the loads were increased by 1.5 times and the following nonlinear capacity analysis of the gate structure was performed.
The system does not collapse even under 1.5 times the load.For the capacity analysis, the force-displacement curve of the reference node number 1321 (Figure 30) is examined in the model, as shown in Figure 31.The loads are gradually increased, considering the force-displacement curve for nonlinear behavior.This analysis shows that the system continues to support the load and does not collapse.According to this curve, the system has not 16 Modelling and Simulation in Engineering collapsed when it is under load and has reached its maximum value.The maximum compressive stress of the concrete is 20 MPa, and the stress distribution is shown in Figure 32 when the hydrostatic load at 85 m is increased by one and a half times.This compressive stress is lower than the maximum strength of the concrete C20/25.On the other hand, it was found that the deformation limits of the concrete were exceeded in some local areas, as can be seen in Figure 33.

Conclusions
In this study, a nonlinear analysis method is used to simulate the real behavior of the structure under hydrostatic loading.

Modelling and Simulation in Engineering
The nonlinear 3D modelling uses C3D8R elements with reduced integration and 8 hexahedral nodes and considers the concrete damage model/concrete damage plasticity model and the tension stiffening model in ABAQUS.The analysis of the limit state collapse should be performed using a nonlinear finite element analysis method that takes into account the real behavior of a composite system and the principle of stress redistribution.
A nonlinear capacity analysis of the gate structure was carried out.The loads were gradually increased up to 1.5 times the hydrostatic forces, and the force-displacement curve was plotted for a reference point in the finite element model.It turned out that the concrete compressive stresses of 20 MPa determined in the calculations were lower than the maximum compressive stress of the concrete, namely, 25 MPa, and that no collapse or crushing of the concrete occurred.On the other hand, the nonlinear capacity analyses and investigations showed that the deformation limits of the concrete were exceeded in some local areas.
In the nonlinear 3D finite element analysis, the anchorages between the concrete of the first and second phases of the gate structure and the steel profiles in the support areas where the gates were subjected to hydrostatic loads are also included according to the project details, considering the construction phases, to obtain the actual load and stress distribution.The results of the analysis showed that the bond behavior of the system with the bonding and the nonlinear behavior of the concrete influenced the results.It was found that these steel anchors carry very large loads and allow the composite system to act with a bond.Therefore, the nonlinear 3D finite element modelling, analysis, and design of the composite system with the modelling of the anchors and steel sections are important for the load transfer of tunnel diversion structures and gates.
Diversion tunnel gates of a dam are the critical part of a dam's safety structures.It is suggested that dam monitoring and control systems can be used to assess and control the gates of a dam according to the water level and water flow rate, monitor the erosion in the tunnel, and control the problems with the advantages of artificial intelligence applications and warning systems.The use of multiple gates is also recommended if a problem occurs in the operation of a gate in the diversion tunnels of a dam to ensure the safety of the tunnel gates in dam structures.
For future studies, the developed model can also be validated by experimental tests with prototypes.The validation of the model is done by checking simple load and stress and strain hand calculations in engineering considering the structural behavior of the tunnel gates observed in the finite element modelling and simulations in this work.The quality of the concrete in the diversion of the tunnel gate of the dam structure was determined based on the core test results of in situ concrete specimens.

Figure 1 :
Figure 1: Structure of the diversion tunnel and gate.

Figure 2 :
Figure 2: View of the diversion tunnel from the dam reservoir.

Figure 4 :
Figure 4: The sections and front view of diversion tunnel gate structure.

Figure 5 :
Figure 5: Detail 1: steel plates and anchor connections in the first and second phases of the concrete.

Figure 6 :
Figure 6: Detail 2: steel plate and anchor connection in the first and second phases of the concrete.

Figure 7 :Figure 8 :
Figure 7: Plate and anchor connection in the first and second phases of the concrete.

Figure 9 :
Figure 9: The thickness of the beam is 250 mm and under the beam where the gate lies.

Figure 13 :
Figure 13: Steel profiles, plates, and anchoring dimensions (for a 2 m long piece).

Figure 15 :
Figure 15: Load and boundary conditions in the ABAQUS model.

Figure 16 :
Figure 16: Boundary conditions of the finite element model.

Figure 17 :
Figure 17: Material models for nonlinear analysis of the concrete.

Figure 19 :
Figure 19: Applied pressure loads to the finite element model.

Figure 20 :
Figure 20: Detail of the sealing at the top of the gate.

Figure 21 :
Figure 21: Lateral supports and load distribution on the gate structure.

Figure 23 :
Figure 23: Maximum compressive stresses (maximum value 13.31 MPa, value in the first and second phases between 5 and 8 MPa).

Figure 24 :
Figure 24: Maximum displacement due to the applied pressure (maximum displacement: 0.2 mm).

13
Modelling and Simulation in Engineering model was assumed to be a fixed bearing.The load and boundary conditions of the structure are shown in Figure 15, and the boundary conditions of the finite element model are shown in Figure 16.The material models for the nonlinear analysis of the concrete and the elastoplastic behavior of steel are shown in Figures 17 and 18, respectively.The ultimate compressive strength of C25 is 25 MPa, and the tensile strength 1.75 MPa

14
Modelling and Simulation in Engineering is used for the nonlinear analysis.The material properties of the concrete (C25), steel sections (St37), and reinforcement (StI) are used for linear and nonlinear analysis (see Table1 ).The modulus of elasticity of the concrete C25 is used with 30000 MPa for the linear analysis and with 23500 MPa in the Popovich model for the nonlinear analysis.The modulus of elasticity of the steel sections (St37) is 206180 MPa and 200000 MPa for the anchor reinforcement.Poisson's ratio is assumed to be 0.2 and 0.3 for concrete and steel, respectively.3.1.Applied Loads and Simple Stress Analysis for Simulation of the Gate Structure.The applied pressure loads as hydrostatic loads are shown in Figure 19.For a simple load and stress control of the gate at a maximum hydrostatic load at a water level of 85 meters, the maximum hydrostatic water pressure on the side surfaces and the concrete top layer, which comes after the plate, is shown in Figure 19 as Q1 and Q2: Q1 = 85 m × 1000 × 9 8 = 833 kPa 1 Load and pressure due to the plate on which each gate stands are as follows: F = 85 m × 8 m × 10 kN/m 3 = 3400 kN,

Figure 33 :Figure 32 :
Figure 33: Deformations at 1.5 times loads for the capacity check.

3
Modelling and Simulation in Engineering

Table 1 :
Material properties used in the finite element analysis.