Fault Analysis of Electric Gate Valve Based on Finite Element Analysis

Abstract

Gate valves operate in harsh environments involving high pressure, high temperature, and high radioactivity over extended periods, making them prone to damage such as yielding, buckling, and fatigue. Therefore, analyzing the structural integrity of gate valves and identifying failure causes is critical. This study uses SolidWorks to model the gate, valve body, and other components, then imports the model into ANSYS for further analysis. The loads under typical operating conditions are computed, boundary conditions are applied, and the ultimate stress is determined for each condition. The resulting stress distribution is compared to relevant standards to evaluate whether the structural integrity meets the required specifications. Finally, the gate valve is disassembled based on the conclusions from the theoretical analysis, and the accuracy of the analysis is verified by comparing the disassembly results with the theoretical predictions.

Introduction

During hot-state testing of the nuclear power primary circuit system, abnormal flow readings in the residual heat removal system were frequently observed. When the residual heat removal system is unavailable, gate valve failure is a primary cause. Rapid and efficient testing, troubleshooting, and fault analysis of gate valves are essential for ensuring safe and stable operations.

Following the nuclear accident at Three Mile Island in the United States, valve fault diagnosis technologies and methods have received increasing attention and made significant progress. Currently, valve fault detection methods primarily rely on algorithms combining wavelet packet transform, empirical mode decomposition, and machine learning. However, these methods are best suited for multi-sample scenarios and are not applicable in cases where limited fault samples are available in real industrial environments. Therefore, accurately diagnosing valve faults when only limited sample data is available has become a critical focus in valve fault detection research. This study applies finite element analysis to model the gate valve and valve body, calculating the ultimate stress of the model under various typical operating conditions. The validity and accuracy of the finite element analysis are confirmed by comparing the disassembly results with the theoretical predictions.

1. Steps for Static Mechanical Analysis of Structures Using the Finite Element Method

1.1 Selection of Appropriate Shape Functions

In finite element analysis, the primary focus is on the displacement, strain, and stress of individual elements, which are related to nodal displacements. When displacement can be represented by a simple function, it is referred to as the shape function. The accuracy of the analysis depends significantly on selecting an appropriate shape function. The relationship between the shape function matrix [N], the nodal displacement matrix [δ]e​, and the displacement matrix [δ]at any point within the element is expressed as:

Where:

• [δ] is the displacement matrix at any point within the element.
• [δ]e​ is the nodal displacement matrix.
• [N] is the shape function matrix.

1.2 Analysis of the Element’s Mechanical Properties

The analysis of an element’s mechanical properties consists of three key parts:

(1) Deriving the relationship between nodal displacement and element strain:

Where:

• [ε] is the strain matrix at any point within the element.
• [δ]e​is the nodal displacement matrix.
• [B] is the strain-displacement matrix.

(2) Establishing the relationship between element stress and nodal displacement:

Where:

• [σ] is the stress matrix at any point within the element.
• [D] is the elasticity matrix for the element material.
• [δ]e​ is the nodal displacement matrix.

(3) Formulating the equation that defines the relationship between nodal forces and displacements (the element stiffness equation):

Where:

• [K] is the element stiffness matrix.
• [F] is the nodal force vector.

1.3 Calculation of Equivalent Nodal Force

Based on the principle of virtual work, external forces acting on an element are replaced by equivalent nodal forces that produce the same virtual displacement. These forces effectively substitute all external loads applied to the element.

1.4 Formulation of the Equilibrium Equation

The equilibrium equation is established by relating the global stiffness matrix [K], the global load vector [F], and the nodal displacement vector [δ]:

1.5 Determination of Structural Displacement and Element Stress

Boundary conditions (necessary constraints) are first applied to eliminate rigid body displacement. The unknown nodal displacements are then calculated using the equilibrium equation with boundary conditions. Finally, the displacement and stress at any point within the element are determined using the shape functions and strain-displacement matrix.

2. Finite Element Model of the Valve Body and Lead Screw, and Meshing

The gate valve was parametrically modeled in SolidWorks and directly imported into ANSYS Workbench for simulation. Using ANSYS Workbench’s computational capabilities, a free meshing method based on tetrahedral elements was employed. Mesh sizes ranging from 1 mm to 50 mm were tested for the gate and lead screw to conduct a convergence analysis, evaluating data trends and computation time. For complex geometries in the gate and lead screw, manual adjustments were made to achieve a target mesh size of approximately 10 mm. A comparison of stress distributions for mesh sizes of 12 mm, 10 mm, and 8 mm indicated that convergence was achieved below 10 mm. While a 10 mm mesh provided reasonable results, further refinement with mesh sizes of 2 mm, 2.5 mm, and 4 mm enhanced accuracy. To optimize computational efficiency and data precision, the gate and lead screw meshes were refined. The final mesh consisted of 320,166 elements with 460,313 nodes. The gate mesh was set to 2.5 mm, while the lead screw was assigned a coarser mesh. Figure 1 illustrates the gate valve mesh generated in SolidWorks.

Figure 1 Grid division of valve plate and lead screw

3. Strength Analysis of Gate Valve Disc

3.1 Determination of Gate and Screw Boundary Conditions

3.1.1 Determination of Opening and Closing Torque

Finite element analysis (FEA) using ANSYS was employed to assess the stress at the T-slot of the gate. The electric gate valve’s gate and seat are designed for single-sided sealing, and as such, the stress calculations were performed under this condition.

3.1.2 Determination of Constraint Conditions

When the gate valve is open, liquid pressure is applied to one side of the valve plate. When the valve is closed, liquid is present on both sides, exerting pressure on both surfaces. In accordance with the gate valve testing requirements, external loads of 4.0 MPa at 20 °C and 14.0 MPa at 240 °C were applied to the valve plate and lead screw plate, respectively. The valve’s opening and closing time was constrained to 22 seconds. The analysis was conducted under static load assumptions, accounting for liquid flow through the valve body and its self-weight. The loading conditions are depicted in Figure 2.

• A fixed constraint was applied at the contact point between the top of the gate plate and the lead screw.
• A self-weight constraint was applied at the lower end of the gate plate.
• Medium pressure (Fa) was applied to one side of the gate plate, with the assumption that the load is evenly distributed across the plate’s surface.
• The resultant clamping force (Fsy) in the Y-axis direction was applied to the lower sealing surface, where the bottom of the gate contacts the valve body.
• A fixed constraint, representing a fluid temperature of 20 °C, was applied to the gate sealing surface.

Figure 2 Valve plate loading position and force diagram

3.2 Finite Element Analysis Under Different Constraints

The results of the finite element analysis are influenced by the applied constraints and loads. To ensure accurate calculations, the constraints and loads were applied according to the specific operating conditions. The analysis was conducted in two stages:

3.2.1 Operating Condition 1

• An upward force of 75,000 N was applied via the pull rod to lift the gate.
• The operating temperature was set to 20 °C.
• A water pressure of 4.5 MPa was applied to one side of the gate tube.
• The gate was constrained by the valve body on both sides, restricting movement perpendicular to the gate surface.
• The operating cycle was assumed to last for 22 seconds.

3.2.2 Operating Condition 2

• An upward force of 75,000 N was applied via the pull rod to lift the gate.
• The operating temperature was set to 240 °C.
• A water pressure of 14 MPa was applied to one side of the gate tube.
• The gate was constrained by the valve body on both sides, restricting movement perpendicular to the gate surface.
• The operating cycle was assumed to last for 22 seconds.

3.3 Stress Analysis of the Gate Using Finite Element

A static finite element analysis of the gate was conducted. The analysis revealed that the maximum equivalent stress on the gate was 149 MPa under low temperature and low pressure, with a shear displacement of 0.17 mm. Under high temperature and high pressure, the maximum equivalent stress increased to 182 MPa, accompanied by a shear displacement of 1.28 mm. At this point, the stress remained within the material's maximum allowable limit. To assess the opening and closing behavior of the T-slot, the valve plate's T-slot area was magnified by a factor of five. The analysis indicated that the valve plate design could benefit from further optimization. Since the valve plate and screw are mating components, both should be optimized concurrently.

3.4 Analysis Conclusion

The equivalent stress contour plot showed that when the evaluated stress of the gate plate's T-slot exceeded the material's allowable stress, the contact surface strength of the T-slot failed to meet the design specifications, resulting in deformation at the center of the four segments of the T-slot.

4. Effect Inspection Based on Gate Valve Disassembly

4.1 Gate Plate Condition After Disassembly

Based on the results of the stress analysis of the valve plate, the failure mode, characterized by separation between the lead screw and the gate plate of the electric gate valve, was identified. This prompted the disassembly and inspection of all electric gate valves. Special tools were utilized during the disassembly process to remove the gate plate. Upon disassembly, circular fractures were observed on the contact surface between the T-slot of the gate plate and the T-head of the lead screw, with pronounced outward deformation at all four corners of the T-slot, as shown in Figure 3.

Figure 3: Macro view of the fracture after valve plate disassembly

4.2 Gate Plate Dimensional Inspection

A vernier caliper was employed to measure the dimensions of the gate plate T-head and the diameters of the upper and lower notches in the T-slot to evaluate deformation in the gate plate.

(1) Comparison of gate plates P1, P2, and P3 showed a general widening trend in the T-slot from bottom to top, with more pronounced deformation observed in the upper section compared to the lower section.

(2) Comparison of gate plates P4 and P5 revealed significant tensile elongation in the T-slot of the gate plate, as shown in Figure 4.

(3) The measurements also indicated that the diameters of the upper and lower notches in the T-slot were larger than the corresponding dimensions of the T-head of the lead screw.

The specific locations and dimensions of the notches in the gate plate T-slot are provided in Table 1.

Figure 4: Measurement diagram of the gate plate T-slot

Table 1: Gate T-slot Notch Size Measurement

Measure the size of the valve plate T-slot, and the data record and drawing requirements are shown in Table 2.

Table 2: Comparison Table of Gate T-slot Data Records and Drawing Requirements

4.3 Screw Size Inspection

A vernier caliper was used to measure the dimensions of the screw. The measurements of the screw T-head are shown in Figure 5. A comparison of the measured dimensions with the drawing specifications is provided in Table 3.

Figure 5: Screw T-head measurement dimensions

Table 3: Comparison of Screw T-head Data Records and Drawing Requirements

The measurement results confirm that the dimensions of the screw T-head and gate T-slot are in compliance with the specified drawing requirements. Initial analysis indicates that the tensile and yield strengths of the screw material are higher than those of the gate material, preventing plastic deformation of the screw during the gate valve's opening and closing cycles. Upon disassembly, the screw and nut were inspected, and the ball and raceway surfaces were found to be clean and in good condition.

4.4 Fracture Mechanism Analysis

• Fracture Analysis: The fracture of the gate T-slot was analyzed in detail.
• Macroscopic Inspection: Upon inspection of the fracture surface and metal fragments, it was observed that the lower surface displayed a bright, silvery white appearance with signs of extrusion and wear, while the upper part was light gray, with fine cross-sections and noticeable plastic deformation. Preliminary findings suggest that cracking initiated at the lower surface of the four-corner boss, where extrusion marks were visible. The interruption zone, showing significant macroscopic plastic deformation, was located on the upper surface of the fracture.
• Microscopic Inspection: The fracture morphology was examined using scanning electron microscopy (SEM). The crack initiated from the lower surface and extended to the upper end of the four corners. Plastic deformation was evident at the fracture edge. Region A was smaller, exhibiting a dimpled morphology with extrusion cracks visible at the fracture edge (Figure 6). Region B was characterized by wear morphology, with some partial dimpled areas ( Figure 7).

Figure 6: Fracture of Region A

Figure 7: Fracture of Region B

4.5 Summary of Inspection Findings

The chemical composition, metallographic structure, inclusions, grain size, α-phase area content, macrostructure, and mechanical properties of the gate plate, including room and high-temperature tensile properties, room temperature impact properties, intergranular corrosion resistance, and hardness, meet the technical requirements for 06Cr18Ni11Ti forgings. Based on these findings, it is concluded that the gate plate T-slot was subjected to high stress, leading to cumulative damage, deformation, and cracking, which ultimately resulted in shear fracture.

5. Conclusion

The gate valve operates under challenging conditions, including high pressure, elevated temperatures, and high radiation levels over extended periods, making it susceptible to failure modes such as yielding, buckling, and fatigue. Therefore, assessing the structural integrity of the gate valve and identifying the root causes of failure are essential. This study investigates the failure mechanisms of an engineering gate valve, utilizing SolidWorks for component modeling and ANSYS for finite element static analysis of the gate plate and lead screw. Two operating conditions of the gate valve were simulated to evaluate the stress distribution of the gate plate. The equivalent stress distribution reveals that the stress in the gate plate T-slot exceeds the material’s allowable stress, and the contact surface strength of the T-slot fails to meet the design requirements, showing signs of deformation.

To validate the findings from the finite element analysis, the valve plate and lead screw were disassembled and inspected. The failure characteristics observed during disassembly, along with the comparison of the valve plate and lead screw before and after the test, confirm that the finite element analysis results align with actual conditions. These findings suggest that both the gate valve plate and the screw may benefit from further structural optimization, which can be verified through post-optimization strength analysis using finite element methods.