Research on the Design and Verification Process of Mechanical Penetrations in Reactor Compartment

Abstract

Mechanical penetrations, as important pressure pipelines penetrating the reactor compartment, withstand high temperatures and pressures. The current complete design and verification process for mechanical penetrations. This article focuses on the problem of stress concentration and easy damage of the penetration components in the reactor compartment under high temperature and high pressure environment. Combining with the existing regulations of nuclear power plants and ships, finite element analysis method is used to analyze the stress of the penetration components under specific high temperature and high pressure and ship ultimate load coupling. At the same time, based on the simulation analysis results, the structural dimensions of the penetration components are optimized, and a mechanical penetration verification process is designed. The coupled thermal stress results of the penetration indicate that the stress of the penetration is too large at the tail of the sleeve, with the values of primary film stress Pm and primary bending stress Pb being 228.2 and 275.91 MPa, respectively. From this, it can be seemed that there is obvious stress concentration at the junction of the support ring and sleeve, as well as at the transition point of the insulation layer, which is the weakest area of the penetration.

1 Introduction

Floating nuclear power plant (FNPP), also known as floating nuclear power plant, is a mobile small nuclear power plant on the ocean. It combines small nuclear reactors with maritime transportation engineering, which can meet the needs of cooling and heating in urban areas, reducing haze weather, and energy supply in remote areas [1]. Mechanical penetrations are part of the reactor containment vessel and are components that connect the internal and external pipelines of the containment vessel [2]. According to the relevant requirements of nuclear safety, mechanical penetrations still need to maintain the ability to perform their functions under severe accident conditions [3].

Mechanical penetrations are installed on the cabin walls to transport fluid inside and outside the cabin. As an important component of the cabin structure, they, together with electrical penetrations, shielding doors, and the main structure of the cabin, form the third barrier for radioactive shielding in the cabin [4]. The penetration is connected to the cabin bulkhead and is located in a structurally discontinuous position, where stress is easily concentrated. Therefore, the structural strength design of the penetration should not only ensure the airtightness and integrity of the safety shell, but also meet the mechanical performance requirements under various working conditions. At present, many experts and scholars at home and abroad have conducted research on it. Li [5] used finite element software ABAQUS to simulate the steady-state and transient thermal coupling of pressure vessels, analyzed the law of coupled thermal stress during radial and circumferential changes in the vessel structure, and explored the influence of temperature on heat transfer; Hazizi [6] combined with ASME specifications and designed a cylindrical pressure vessel that will not fail by analyzing a pressurized liquefied petroleum gas vertical pressure vessel with a capacity of 10 cubic meters. Jasion [7] studied a pressure vessel with a special cylindrical shape, established an analytical model of this container composed of a rotating shell, and based on membrane theory, analyzed, and determined the stress state in the container. Chen [8] designed a set of loading test equipment to meet the testing requirements of penetrations under extreme load. It was found that when the ultimate load was applied, the stress was mainly concentrated at the root of the penetration; Tong [9] analyzed the stress and deformation of the containment vessel, as well as its ultimate bearing capacity, using a prestressed finite element model. Song [10] conducted vulnerability analysis and probabilistic safety performance evaluation of the nuclear containment structure under the condition of prestressed tendon fracture based on the finite element model of the nuclear containment. They discussed the changes in concrete compressive stress state and the ultimate bearing capacity of the nuclear containment structure, and analyzed the vulnerability curve and probabilistic safety margin of the nuclear containment structure under the condition of prestressed tendon fracture.

Currently, there are complete regulations in domestic and foreign regulations regarding the evaluation standards for nuclear grade pressure vessels. However, there is no clear regulation on the design verification process and evaluation standards for nuclear grade pressure vessels on ships, such as mechanical penetrations in storage tanks. Therefore, this study combines ships with nuclear power plants. Based on the relevant specifications of nuclear grade pressure vessels and ship structures, combined with theoretical research and specific engineering examples, finite element software is used to conduct thermal coupling simulation analysis on the penetration components of the reactor compartment. Based on the results, the structural dimensions of the penetration components are optimized, and a set of process verification methods is designed. In this paper, a reactor tank penetration with a size of φ 273.0 × 25.4 [11] was designed and checked through thermal simulation and stress deformation simulation analysis and calculation.

2 Thermodynamic Coupling Theory

The coupling field can be divided into different physical fields: magnetic field and electromagnetic field, magnetic field and stress field, temperature field and stress field, temperature field and flow field coupling, etc. The coupling methods are divided into direct coupling and sequential coupling. Direct coupling involves introducing coupling effects into the control equation through element matrices or load vectors, and then solving the control equation. The calculation process is convenient but the calculation accuracy is not high, and it is mostly suitable for theoretical analysis of coupled fields; Sequential coupling is the process of solving a single physical field within each incremental step, and then applying the solution of the previous physical field as an external load to the latter physical field to complete the coupling of the two physical fields. Although the calculation process is relatively complex, this method has high computational accuracy and is suitable for engineering calculations of coupled fields [12].

This article adopts the sequential coupling method, and the finite element equation of sequential coupling is:

$$\left[\begin{array}{ll}{K}_{11}{X}_{1}+{K}_{11}{X}_{2}& 0\\ 0& {K}_{22}{X}_{1}+{K}_{22}{X}_{2}\end{array}\right]\left\{\begin{array}{l}{X}_{1}\\ {X}_{2}\end{array}\right\}=\left\{\begin{array}{ll}{F}_{1}{X}_{1}+{F}_{1}{X}_{2}\\ {F}_{2}{X}_{1}+{F}_{2}{X}_{2}\end{array}\right\}$$

(1)

In the formula: ${X}_{1}$ and ${X}_{2}$ represent the displacement matrices of two physical fields; ${F}_{1}$ and ${F}_{2}$ represent the equivalent load matrices of two physical fields; ${K}_{11}$ and ${K}_{22}$ represent the equivalent stiffness matrices when two physical fields exist separately.

Bring the single stress field control equation and the single temperature field control equation into the sequential coupling control equation to obtain the thermal coupling control equation:

$$\left[\begin{array}{ll}M& 0\\ 0& 0\end{array}\right]\left\{\begin{array}{l}\ddot{u}\\ \ddot{T}\end{array}\right\}+\left[\begin{array}{ll}C& 0\\ 0& {C}^{t}\end{array}\right]\left\{{\begin{array}{l}{\dot{u}}\\ {\dot{T}}\end{array}}\right\}+\left[\begin{array}{cc}K& 0\\ 0& {K}^{t}\end{array}\right]\left\{\begin{array}{l}u\\ T\end{array}\right\}=\left\{\begin{array}{l}F\\ Q+{Q}^{p}\end{array}\right\}$$

(2)

In the formula: $u$ and $T$ are the element displacement matrix and element temperature matrix, respectively; $C,{C}^{t}$ is the unit damping matrix and the unit specific heat matrix, respectively; $K,{K}^{t}$ is the element stiffness matrix and the element heat conduction matrix, respectively; $M$ is the unit quality matrix; $F$ is the unit load matrix; $Q$ is the unit heat generation and unit heat flow rate; ${Q}^{p}$ is the unit plastic heat generation rate.

When the temperature of the penetration changes, deformation will occur, resulting in thermal stress in the structure. The thermal stress of high-energy penetration belongs to secondary stress, which needs to be considered under various working conditions. Therefore, the strength of the penetration must meet the requirements under ultimate load. At the same time, in order to ensure that the temperature of the shielding material is within its working temperature range, thermal coupling analysis of the penetration is necessary. This article uses Ansys software and sequential coupled thermal analysis method to calculate the stress components of each component of the penetration, and verifies the strength of each component of the penetration according to the stress assessment criteria of ASME code [13]. The flow chart of the sequential coupled thermal analysis method in this article is shown in Fig. 1.

Fig. 1

Thermal analysis method process

3 Model and Mesh

A certain reactor compartment is 1 m × 1 m × 1 m enclosed space, pipeline penetrations are key components for fluid transportation inside and outside the reactor compartment, mainly including structural parts and other ancillary structures. The geometric model of the penetration is 1 m × 1 m × 1 m 3D model including the penetration. The structure of the penetration includes the middle pressure pipe, the head between the pipe and the sleeve, the sleeve and the support ring; The remaining components are auxiliary structures, including the insulation layer between the sleeve and the penetrating pipe fittings, fixed steel bars, angle steels, and resin plates, radiation resistant materials such as lead plates and lead boron polyethylene, and fire-resistant materials such as polycrystalline wires; The rest is filled with air. The three-dimensional model of the penetration is shown in Fig. 2.

Fig. 2.

3D geometric modeling of penetration

The geometric grid size of the bulkhead and T-shaped support plate is set to 15 mm, the web plate is set to 10 mm, the bar steel, angle steel, and resin plate are set to 5 mm, and the polycrystalline wire is set to 7.5 mm. For penetrations, sleeves, and support rings, the grid size is set to verify the thickness direction of three units. For welding points, the grid size is set to 1 mm, and for other areas, the grid size is set to default. At the same time, select slow transition areas for the grid transition, set the resolution for small areas to 3, and the number of grid cells is 6,865,833. The 3D mesh model is shown in Fig. 3.

Fig. 3

Mesh division of penetrations

4 Boundary Condition

4.1 Temperature Field Boundary Conditions

The interior of the penetration pipe is a high-temperature and high-pressure fluid. During the steady-state simulation of the temperature field of the penetration and its affiliated structures, the inner wall of the penetration pipe is assumed to be convective heat transfer. When the internal fluid is liquid, the convective heat transfer coefficient is taken as 2000 w/m² K, and when the internal fluid is gas, the convective heat transfer coefficient is taken as 300 w/m² K, with an ambient temperature of 25 ℃ and a convective heat transfer coefficient of 15 w/m² K; The bulkhead and T-shaped support platform are connected to the storage tank as an insulated wall surface; The contact between other external surfaces and the environment is assumed to be natural convection, and the internal fluid is set as gas. The specific boundary conditions are set as shown in Fig. 4.

Fig. 4

Setting of temperature boundary conditions for penetrations

4.2 Stress Field Boundary Conditions

The loads borne by the penetration are mainly the design internal pressure, temperature load, and nozzle load. The design internal pressure is set as surface pressure, which acts on the inner wall of the connecting piece along the internal normal direction, at a pressure of 7.0 MPa; There are two commonly used methods for determining the nozzle load of nuclear vessels: ① conducting mechanical analysis of the pipeline system to obtain the nozzle load of the vessel; ② The allowable load of the nozzle (which is the upper limit value of the nozzle load obtained from the mechanical analysis of the pipeline system) is determined based on the geometric parameters, material characteristics, force torque relationship, and stress assessment criteria under various load conditions of the container nozzle. Method ② is not affected by the progress of piping analysis. In the preliminary stage of nuclear vessel design, in order to accelerate the engineering progress, a container-based nozzle load analysis method can be used.

According to the provisions of Section III of the ASME Boiler and Pressure Vessel Code and the Construction Rules for Nuclear Facility Components, the allowable nozzle load of the vessel is calculated to ensure that the maximum stress caused by the design pressure and external load does not exceed the limit of primary stress under design, critical, and accident conditions. Therefore, based on the geometric parameters and material characteristics of the nozzle structure, the stress intensity values at each section of the nozzle can be obtained. Then, according to the overall primary membrane stress intensity P_m, local primary membrane stress intensity P_L, P_m (or P_L) + primary bending stress intensity P_b stress limit value specified in the ASME code under various working conditions, the allowable nozzle load can be determined by calculating the assumed nozzle load of each type [14]. According to elasticity, the stress calculation of the evaluated section is as follows:

Axial stress:

$${\sigma }_{z}=\frac{P}{A}+\frac{{p}_{{\text{i}}}{r}_{{\text{i}}}}{2t}+\frac{{M}_{{\text{B}}}{r}_{{\text{o}}}}{I}$$

(3)

In the formula: ${p}_{{\text{i}}}$ is the internal pressure, Pa; $A$ is the cross-sectional area, m²; ${r}_{{\text{i}}}$ is the inner radius, m; ${r}_{{\text{o}}}$ is the outer radius, m; $t$ is the wall thickness, m; $I$ is the moment of inertia, m⁴; ${M}_{{\text{B}}}$ is the total bending moment, N m.

Circumferential stress:

$${\sigma }_{0}=\frac{{p}_{{\text{i}}}{r}_{{\text{i}}}}{t}$$

(4)

Radial stress:

$${\sigma }_{r}=-\frac{{p}_{{\text{i}}}}{2}$$

(5)

Shear stress:

$$\begin{array}{c}\tau ={\tau }_{1}+{\tau }_{2}\\ {\tau }_{1}=\frac{VQ}{2It};{\tau }_{2}=\frac{{M}_{1}{r}_{0}}{2I}\end{array}$$

(6)

In the formula: Q is the shape coefficient, m³.

Section 3 principal stresses ${\sigma }_{1}$, ${\sigma }_{2}$, ${\sigma }_{3}$ is:

$$\begin{array}{c}{\sigma }_{1}=\frac{{\sigma }_{z}+{\sigma }_{\theta }}{2}+{\left[{\left(\frac{{\sigma }_{z}-{\sigma }_{\theta }}{2}\right)}^{2}+{\tau }^{2}\right]}^{0.5}\\ {\sigma }_{2}=\frac{{\sigma }_{z}+{\sigma }_{\theta }}{2}-{\left[{\left(\frac{{\sigma }_{z}-{\sigma }_{\theta }}{2}\right)}^{2}+{\tau }^{2}\right]}^{0.5}\\ {\sigma }_{3}={\sigma }_{r}\end{array}$$

(7)

The stress difference on the section is:

$$\begin{array}{c}{S}_{12}=\left|{\sigma }_{1}-{\sigma }_{2}\right|\\ {S}_{23}=\left|{\sigma }_{2}-{\sigma }_{3}\right|\#\\ {S}_{13}=\left|{\sigma }_{3}-{\sigma }_{1}\right|\end{array}$$

(8)

The total stress intensity is:

$${S}_{{\text{I}}}={\text{max}}\left({S}_{12},{S}_{23},{S}_{13}\right)$$

(9)

In solid mechanics simulation, the outer wall and connecting plate are set as fixed constraint points, and the nozzle load is calculated according to the formula, which is divided into four types: Tensile force F_T = 253.652 kN; Shear force F_V = 253.652 kN; torque M_V = 126.826 kN m, and Bending moment M_B = 126.826 kN m. The torque is clockwise. Due to the connection between both ends of the penetration and the connecting pipeline, four types of nozzles load under normal operating conditions are applied at both ends of the penetration. The loading method is shown in Fig. 5.

Fig. 5

Setting of mechanical boundary conditions for penetrations

5 Calculation and Result Analysis

After setting the boundary conditions, conduct a steady-state analysis and solution of the temperature field of the penetration; Import the temperature field into the mechanical analysis interface for thermal stress analysis, and then load the mechanical boundary conditions again to enter the stress evaluation analysis.

There are two main verification standards for temperature field simulation: 1. Whether the maximum temperature of the lead plate shielding layer exceeds 300 ℃; 2. Does the maximum temperature of the lead boron polyethylene shielding layer exceed 120 ℃.

For the stress field, set the stress path and extract the membrane stress and bending stress on the stress path. The stress path is shown in Fig. 6.

Fig. 6

Penetration stress path

Calculate the allowable stress of different components according to the specifications, verify each stress component according to the allowable stress, and complete stress assessment. The stress assessment criteria for penetrations are shown in Table 1.

Table 1 ASME evaluation standards

5.1 Temperature Field Evaluation

The temperature field distribution of the penetration after steady-state temperature simulation is shown in Figs. 7, 8 and 9. The overall maximum temperature of the penetration is 299.4 ℃, and the minimum temperature is 25.151 ℃; The maximum temperature of the lead plate shielding layer is 29.103 ℃, and the minimum temperature is 26.044 ℃; The maximum temperature of the lead boron polyethylene shielding layer is 58.226 ℃, and the minimum temperature is 26.157 ℃. The calculation results indicate that the temperature evaluation of the penetration meets the design requirements.

Fig. 7

Overall temperature distribution of penetration

Fig. 8

Temperature distribution of lead plate shielding layer

Fig. 9

Temperature distribution of lead boron polyethylene shielding layer

5.2 Stress Field Evaluation

The stress field distribution of the penetration after steady-state stress simulation is shown in Fig. 10. The maximum overall stress of the penetration is 651.44 MPa, and the stress is mainly concentrated at the root.

Fig. 10

Overall stress distribution of penetrations

According to ASME Section II specifications, compare the calculated stress components with the corresponding allowable stresses. Under normal working conditions, take a 90° profile stress, and the evaluation results are shown in Table 2. The calculation results show that the stress of the penetration is at paths 11 and 12, with the values of primary membrane stress P_m and primary bending stress Pb being 228.2 and 275.91 MPa respectively, which do not meet the evaluation requirement of 207 MPa. The local stress component of the penetration is relatively large, mainly concentrated at the transition between the insulation layer and the support ring of the penetration. The thickness of the sleeve can be increased to strengthen it.

Table 2 Profile stress assessment results

5.3 Verification Process for Overall Design of Penetrations

For the overall design verification of mechanical penetrations, based on the theory of thermal coupling, the ultimate load calculation is combined with the ASME “Boiler and Pressure Vessel Code” Section III and “Nuclear Facility Component Construction Rules”. The evaluation criteria are in accordance with ASME Section II specifications, and a complete set of processes is designed. The specific design verification process is shown in Fig. 11.

Fig. 11

Verification process for overall design of penetrations

6 Conclusion

This article focuses on the problem of stress concentration and easy damage of the penetration components in the reactor compartment under high temperature and high pressure environment. Combining with the existing regulations of nuclear power plants and ships, finite element analysis method is used to analyze the stress of the penetration components under specific high temperature and high pressure and ship ultimate load coupling. At the same time, based on the simulation analysis results, the structural dimensions of the penetration components are optimized, and a mechanical penetration verification process is designed. Based on the above results, the following conclusions can be drawn:

• (1) The design of the penetration meets the requirements of temperature assessment, but its stress is too concentrated at the junction of the support ring and sleeve, as well as at the transition with the insulation layer, which does not meet the stress assessment requirements. In this regard, the thickness of the sleeve can be increased to allow it to withstand greater stress at the junction with the support ring and insulation layer, in order to optimize the penetration structure and meet the stress assessment requirements.

• (2) When designing and verifying penetrations, first determine the structural model of the penetration, then set the geometric dimensions of the penetration, and select materials based on the specific engineering environment; Calculate the ultimate load according to the formula and conduct thermal coupling analysis on the penetration; At the same time, establish a three-dimensional model, use finite element software to simulate the temperature and stress fields, and finally evaluate based on relevant standards. Based on the evaluation results, optimize the structure of the penetration to meet the design requirements.