A numerical simulation method for high-pressure steam condensation in a pipeline

Abstract

The application discloses a numerical simulation calculation method for high-pressure steam condensation in a pipeline, designs a pipeline model meeting the thermodynamic requirements of a passive residual heat removal system on the secondary side of a pressurized water reactor, establishes a three-dimensional geometric model, divides the three-dimensional geometric model into three blocks corresponding to a steam flow field, a heat transfer pipe field and a cooling water flow field, and further divides the grid, selects a suitable multiphase flow model, a turbulence model and a phase change model, defines material physical properties, sets calculation working conditions, phase interaction and boundary conditions, sets spatial discrete methods of different physical quantities, performs pressure-velocity coupling calculation, sets flow Nusselt numbers, adjusts explicit relaxation factors and sub-relaxation factors, initializes the temperature and pressure of the steam flow field and the cooling water flow field and the temperature of the heat transfer pipe field, starts calculation, adjusts the relaxation factor according to residual fluctuation, exports data, judges the flow state of the steam according to the thermodynamic data of the inner wall nodes of the heat transfer pipe and in combination with a volume fraction cloud chart, and ensures that the thermodynamic requirements of the passive residual heat removal system on the secondary side are met.

Description

Technical Field

[0001] This invention belongs to the field of nuclear reactor safety analysis technology, specifically relating to a numerical simulation calculation method for high-pressure steam condensation in pipelines. Background Technology

[0002] Passive Power Residue Harness (PSHR) systems play a crucial role as key safety facilities ensuring effective removal of residual heat after an accident. Utilizing natural physical phenomena, this system transfers and dissipates heat without the need for an external power source, significantly reducing the risks and complexities of post-accident handling. In the event of an accident, a direct-flow steam generator rapidly produces a large amount of superheated steam. This high-temperature, high-pressure steam is then guided into the heat transfer tubes of the condenser, where the outer walls of the tubes directly contact the cooling medium in the cooling water tank. Through an efficient heat exchange process, the heat released by the steam is transferred to the water in the cooling water tank, causing the steam to gradually condense into liquid water, thus achieving the removal and dissipation of residual heat.

[0003] Within the safety analysis framework of the PSHR (Power Supply Refrigerant Regulator), in-depth research into the condensation mechanism of steam condensation within heat transfer tubes is indispensable. This involves a thorough understanding of complex physical phenomena such as steam condensation behavior on the inner wall of the heat transfer tubes, heat transfer efficiency, flow characteristics of the condensate film, and potential phase change kinetics. These studies not only help optimize condenser design and improve waste heat removal efficiency but also provide a scientific basis for preventing potential condensation failures or insufficient heat exchange.

[0004] Furthermore, the impact of ocean motion conditions on the steam condensation process cannot be ignored. Ocean activities such as waves, tides, and ship navigation can cause vibrations, displacements, or temperature fluctuations in the condenser and its surrounding structures, thereby affecting the stability of the heat transfer tubes and the condensation efficiency. Therefore, in-depth analysis of the steam condensation process under ocean motion conditions is particularly important. This includes assessing the specific impact of different ocean motion parameters on the condenser's heat transfer performance, and exploring possible mitigation measures, such as enhancing structural stability, optimizing the condenser layout, or adopting advanced vibration reduction technologies, to ensure the reliable operation of the PSHR in complex ocean environments.

[0005] In summary, the safety analysis of passive residual heat removal systems (PSHR) requires not only a deep understanding of the basic mechanism of steam condensation within the heat transfer tubes, but also full consideration of the various impacts that ocean motion conditions may have on the condensation process, thereby providing solid technical support for the safe operation of the reactor. Summary of the Invention

[0006] To address the aforementioned problems, this invention provides a numerical simulation method for high-pressure steam condensation within pipelines. Given the thermal-hydraulic parameters of the inlet steam, the main parameters and states of heat exchange and flow within the pipeline can be calculated, and the heat transfer performance of the heat transfer tubes can be evaluated, providing data for the design of a passive waste heat removal system on the secondary side.

[0007] To achieve the above objectives, the present invention adopts the following technical solution: A numerical simulation method for high-pressure steam condensation in pipelines includes the following steps: Step 1: Design a pipe model that meets the thermodynamic requirements of the passive waste heat removal system on the secondary side of the pressurized water reactor.

[0008] The C-type heat exchanger in the passive waste heat removal system on the secondary side adopts a shell-and-tube condenser design. Due to the high steam temperature and pressure at the inlet, conventional pipe materials are difficult to meet the long-term use requirements. In order to meet the requirements of temperature resistance, pressure resistance and heat transfer, the internal steam channel heat transfer tube is made of Inconel 690 nickel-based high-temperature alloy tube with a diameter of 29 mm × 5 mm and a length of 5000 mm. The maximum long-term operating temperature can reach 1100 ℃, and the maximum pressure at this tube diameter is greater than 20 MPa. The thermal conductivity is about 10~14 W / (m·K) in the temperature range from room temperature to 500K. The external cooling jacket is made of 316L tube with a diameter of 55 mm × 5 mm and a length of 5000 mm.

[0009] Step 2: Based on the dimensions of the pipe model, use SpaceClaim software to create a three-dimensional geometric model.

[0010] Step 3: Use ICEM software to divide the 3D geometric model into three blocks, corresponding to the steam flow domain, heat transfer pipe domain and cooling water flow domain respectively, and then mesh each block.

[0011] When meshing, each block needs to be divided into O-blocks. O-block is the core topology operation in ICEM for structured hexahedral meshes. It is specifically used to handle curved surfaces or axisymmetric geometries such as circles, cylinders, and spheres. It divides the original square blocks into "O-shaped" topologies around the center, which greatly improves the mesh quality near the curved surfaces.

[0012] Because the normal velocity and temperature exhibit a very large gradient near the wall, within a very small distance from the wall, the velocity rises from rest relative to the wall to the mainstream velocity, and the fluid temperature rises from the temperature of undersaturated water to that of saturated steam or even superheated steam. Therefore, two methods are commonly used to calculate the flow field in this region: one is using the wall function method; the other is refining the mesh and using the wall model method to solve for the viscous sublayer. Since steam condensation and heat transfer almost entirely occur at the wall, the mesh near the wall is crucial for the simulation. Therefore, the method of solving for the viscous sublayer is chosen, and mesh refinement is performed near the inner and outer pipe walls in both the steam and cooling water flow domains. y + <1 and close to 1, the boundary layer mesh is divided in the fluid domain on both sides of the heat transfer tube.

[0013] Step 4: Select the appropriate multiphase flow model, turbulence model, and phase change model.

[0014] To better simulate the flow and heat transfer process of high-pressure steam condensing in a pipe, the Mixture model was used for multiphase flow, the SST k–ω model for turbulence, and the Lee model for phase change. The VOF model excels at capturing clear gas-liquid interfaces, but its computational grid requirements are extremely high, and its ability to handle phase changes and dispersed small droplets is not efficient enough. In the Eulerian model, strong interphase momentum exchange requires precise allocation of source terms to the equations of each phase; improper handling can easily lead to imbalances and divergences. The Mixture model can well simulate the flow pattern of a continuous liquid film phase with discrete droplet phases, showing improved stability compared to the VOF model and faster computation speed compared to the Eulerian model. The k–ω model exhibits high accuracy in the viscous sublayer and transition region, requires no complex wall functions, and can be directly integrated to the wall. The k–ε model is more robust in free shear flow far from the wall and in fully developed turbulent regions, and is insensitive to free-flow turbulence values. The SST k–ω model combines the advantages of both, exhibiting a k–ω model in the near-wall region (inner boundary layer) and transforming into a modified k–ε model in the outer boundary layer and free flow. The Lee model determines whether a phase transition occurs based on the temperature difference between the saturation temperature and the working fluid temperature, treating the temperature of the gas-liquid interface as the saturation temperature. When the interface temperature is lower than the liquid phase temperature, evaporation occurs; when the interface temperature is higher than the liquid phase temperature, condensation occurs. The Lee model overcomes the limitations of the phase interface and is the most commonly used phase transition model for condensation simulation, as well as the default phase transition model in Fluent.

[0015] Step 5: Define material properties, set calculation working conditions, phase interactions and boundary conditions. When calculating ocean conditions, a user-defined function (UDF) to control gravity changes also needs to be set.

[0016] High-pressure steam is set as the main phase, and high-pressure condensate, cooling water, and their gas phases as secondary phases. The density, specific heat, thermal conductivity, and dynamic viscosity of each phase at different temperatures are obtained by consulting the REFPROP fluid thermodynamics and transport properties database. Using the saturation temperature as a reference, the standard enthalpy of the liquid phase is set to 0, and the standard enthalpy of the gas phase is set to the same value as the latent heat of vaporization. The mass transfer mechanism from the high-pressure liquid phase to the high-pressure gas phase is set as evaporation-condensation, and the condensation relaxation coefficient is set to 10-500 based on the steam flow rate.

[0017] To ensure proper heat transfer, shadow surfaces must be established on the inner and outer walls of the heat transfer tubes. These shadow surfaces primarily handle the mesh interface between adjacent regions and are closely related to mesh continuity, data transfer, and computational accuracy. If Fluent cannot automatically generate shadow surfaces, two surfaces sharing a common node in different domains on the inner or outer wall must be merged into a new geometry using Boolean operations to automatically generate the shadow surfaces. Since the cooling water temperature is not significantly different from the ambient temperature, the outer casing is set as an adiabatic wall to reduce computational complexity. Velocity inlets are only suitable for incompressible flows, while mass inlets are only suitable for compressible flows. In waste heat removal systems, the steam inlet Mach number is generally no higher than 0.01, considered incompressible flow, therefore a velocity inlet is chosen. Turbulence parameters are set according to the hydraulic diameter and turbulence intensity; default settings or medium turbulence are sufficient. Pressure outlets are most commonly used, allowing pressure to develop freely at the outlet. Fluid recirculation settings are crucial for potential condensate recirculation at the condenser end; the recirculation direction should be set to Normal to Boundary, and low turbulence intensity is recommended for recirculation turbulence.

[0018] When the system operates in the ocean, it will experience six degrees of freedom of spatial motion. These motions mainly have two effects on the nuclear power system: 1) The tilting and rolling motion of the hull will cause changes in the spatial position of pipelines and equipment in the reactor system, resulting in changes in the effective height difference between the heat source and the cold source, which in turn affects the system's natural circulation capability; 2) The undulating and rolling motion of the hull will introduce additional accelerations such as periodically changing tangential acceleration, centripetal acceleration and Coriolis acceleration. The additional acceleration parallel to the flow direction will generate additional pressure drop on the fluid, causing periodic flow fluctuations or drift in the system.

[0019] For both static tilting and undulating motions in ocean conditions, a formulaic gravity setting is used to simulate the motion. However, in oscillating motion, the fluid moves within the pipe in a rotating non-inertial reference frame, generating inertial forces such as the Coriolis force. Therefore, a UDF is needed to precisely control the motion in different directions and to add inertial forces to the oscillating motion.

[0020] User-defined functions (UDFs) are library functions written in standard C and compiled into the Fluent solver. During computation, this code is dynamically loaded and executed to define complex boundary conditions, define custom material properties, specify source terms, initialize the flow field, adjust calculations after each iteration, define custom scalar transport equations, and handle moving meshes. UDF functions are defined based on official macros that begin with "DEFINE_", which are invoked and executed using data obtained from the solver. UDFs are used to supplement standard CFD software when it cannot meet customer needs.

[0021] Step 6: Set up spatial discretization methods for different physical quantities, and use the COUPLED method in Fluent to perform pressure-velocity coupled calculations.

[0022] The COUPLED method is chosen to handle the coupling relationship between velocity and pressure, which is particularly suitable for situations where variables are interrelated in various conservation equations, helping to improve the stability and convergence of the solver during equation solving. During the discretization of the governing equations, the momentum, energy, and species transport terms are expressed in a second-order upwind scheme to improve numerical accuracy, while the pressure term interpolation uses a volume force weighting scheme from Fluent to improve simulation results under natural convection or gravity-driven scenarios. Furthermore, in the calculation of variable gradients, a cell-based Green-Gaussian method is employed to enhance the ability to capture the changing trends of variables in unstructured meshes.

[0023] Step 7: Set the flow Coulomb number and adjust the explicit relaxation factor and the sub-relaxation factor.

[0024] The flow Coulomb number is set to 1, and other relaxation factors are: pressure relaxation factor is set to 0.3, momentum relaxation factor is set to 0.2, energy relaxation factor is set to 0.5, volume fraction relaxation factor is set to 0.1, and turbulence relaxation factor is set to 0.5. The pressure, momentum, and energy relaxation factors can be adjusted appropriately according to the changes in the residual curve.

[0025] Step 8: Initialize the settings for temperature, pressure, and flow rate of the steam and cooling water domains, as well as the temperature of the heat transfer tube domain.

[0026] Step 9: Start the calculation and adjust the relaxation factor appropriately according to the residual fluctuation to stabilize the flow.

[0027] The core principles for setting the flow Coulomb number and other sub-relaxation factors are: starting small and gradually increasing, dynamic adjustment, and coordinating coupled solutions with adaptive time steps. Steam condensation involves a two-phase phase transition between gas and liquid, and the parameter gradient near the wall is extremely high, requiring high numerical stability and strict control of the Coulomb number and relaxation factor.

[0028] If the residual curve decreases slowly, the pressure, momentum, or energy relaxation factor can be increased by 0.1; if the curve fluctuates continuously, it needs to be decreased by 0.1; if the calculation diverges, it needs to be decreased by 0.2 or even more until the calculation converges.

[0029] Step 10: Export solution data. Based on the thermodynamic data of the nodes on the inner wall of the heat transfer tube and combined with the volume fraction cloud map, determine the flow state of the steam to ensure that the thermodynamic requirements of the passive waste heat removal system on the secondary side are met.

[0030] Compared with the prior art, the present invention has the following advantages: Step 1, for the Huakun-1 Science and Technology Demonstration Project, designed a heat transfer pipeline suitable for the passive residual heat removal system on the secondary side of the ACPR50S compact pressurized water reactor. This lays a solid foundation for exploring the steam condensation mechanism within the condenser heat transfer tubes under static and different ocean motion conditions, and for developing or verifying a condensation heat transfer model applicable to high-pressure conditions after the PSHR is put into operation. Closely focusing on the two core aspects of nuclear safety reliability and engineering application accuracy, it provides key technical support for the operational characteristics and safety analysis of the passive residual heat removal system. Furthermore, current research on pipeline steam condensation is mostly limited to the medium and low pressure range, and its models and conclusions are difficult to apply to the high-pressure conditions of nuclear power plants, small modular reactors, and other systems. Conducting simulation research on high-pressure steam condensation within pipelines can reveal the unique mechanism of steam condensation under high pressure, improve the high-pressure phase change and thermo-hydraulic coupling model, significantly improve the simulation accuracy of high-pressure steam systems, and provide more reliable theoretical and methodological support for the thermal design, safety analysis, and life assessment of next-generation nuclear energy systems. This has significant academic value and cutting-edge engineering application potential.

[0031] 2. In step 4, to better simulate the flow and heat transfer process of high-pressure steam condensation in the pipe, the Mixture model is used as the multiphase flow model. Steam condensation in a pipe typically involves a continuous gas phase (steam) and a discrete liquid phase (condensate droplets / liquid film). The Mixture model assumes that each phase moves at the same velocity in a local region, which is more consistent with the characteristics of droplets being carried by the airflow or the liquid film on the wall being dominated by shear force in the early stage of steam condensation. The gas phase is continuous and occupies the dominant volume fraction. Compared to the more complex Eulerian model, which requires solving the momentum and energy equations for each phase, the Mixture model only solves one set of momentum, continuity, and energy equations for the mixed phase, and then solves the volume fraction equations for the secondary phases. This significantly reduces computational resources and time costs, which is very advantageous for common pipe condensation simulations, especially long pipes. The VOF model excels at capturing clear gas-liquid interfaces, but it requires extremely high computational meshes (high resolution is needed at the interface), is very costly, and is not as convenient and efficient as the Mixture or Eulerian models in handling phase changes and dispersed small droplets. Therefore, Mixture achieves the best balance between computational efficiency, good support for phase change, and meeting the accuracy requirements of typical pipeline condensation conditions.

[0032] 3. In step 4, to better simulate the flow and heat transfer process of high-pressure steam condensation within the pipe, the SST k–ω model is used as the turbulence model. The SST k–ω model combines the high accuracy of the k–ω model in the viscous sublayer and transition zone with the robustness of the k–ε model in the mainstream region far from the wall. The condensate forms a liquid film at the wall, and its flow is strongly influenced by wall shear forces. The SST k–ω model accurately captures the flow characteristics and shear stress of the near-wall boundary layer, which is crucial for predicting liquid film thickness, flow state, and their impact on heat and mass transfer. The SST k–ω model has better resolution of the near-wall thermal boundary layer, providing more accurate predictions of the wall temperature gradient and heat flux density, which is critical for calculating the condensation heat transfer rate. Compared to the Standard k–ω model, which is highly sensitive to inlet free-flow turbulence parameters and may lead to unreasonable calculation results, the SST k–ω model introduces a systematic interpretation of k–ε through a mixing function, reducing sensitivity to external turbulent boundary conditions and improving stability. The SST k–ω model has been widely validated in industry and academia for applications involving heat transfer, separated flows, and complex geometries, including condensation heat transfer problems, and is the recommended “advanced” RANS model.

[0033] 4. In step 5, for the two motions of static tilting and undulating motion in ocean conditions, the varying gravitational acceleration can be directly input into Fluent. However, in the oscillating motion, the liquid's motion within the pipe is in a rotating non-inertial reference frame, generating inertial forces such as the Coriolis force. Fluent cannot meet the simulation requirements, so a UDF is used to supplement it, precisely controlling the motion in different directions and adding inertial forces under oscillating motion. During the steam condensation process within the pipe, the negative values ​​obtained by multiplying the sum of centripetal acceleration, tangential acceleration, and Coriolis acceleration in different directions by the fluid density are compiled through the UDF and loaded as mass source terms into the discretized conservation equations.

[0034] 5. In step 6, the COUPLED method is used to couple the solver to handle pressure-velocity coupling, which is suitable for the characteristics of strong multi-physics field correlations in steam condensation, effectively improving solution stability and convergence. The momentum, energy, and composition equations are discretized using a second-order upwind scheme to reduce numerical dissipation and improve computational accuracy. The pressure term uses a volume force weighted interpolation scheme, which is more suitable for the gravity-driven and natural convection flow characteristics of passive waste heat removal systems. The variable gradient calculation uses a cell-based Green-Gaussian method to enhance the ability to capture changes in unstructured meshes and near-wall variables. At the same time, the robust convergence of strongly nonlinear problems is ensured by reasonably setting relaxation factors. The entire solution strategy takes into account accuracy, stability, and engineering applicability, and can more reliably and accurately simulate the flow and heat transfer process of high-pressure steam condensation in pipes, providing an advanced and standardized numerical solution scheme for the thermal-hydraulic analysis of passive waste heat removal systems.

[0035] 6. In step 10, by exporting the complete CFD solution data, based on the high-precision thermodynamic parameters at the node level of the heat transfer tube inner wall, and combined with the gas-liquid integral cloud map, the steam condensation flow state is jointly judged, and finally, it is verified whether the thermodynamic requirements of the passive waste heat removal system on the secondary side are met. This method realizes the mutual verification between local fine quantitative data and global visualized flow patterns, avoiding the errors caused by traditional averaging analysis, and can more accurately identify condensation flow patterns, liquid film distribution, and heat transfer intensity. At the same time, the simulation results are directly benchmarked against the safety functional requirements of the passive waste heat removal system, forming a complete technical closed loop from numerical calculation to system performance evaluation, significantly improving the scientific nature and engineering application value of flow state judgment, and providing advanced and reliable analytical methods for the thermal design and safety analysis of passive waste heat removal systems. Attached Figure Description

[0036] Figure 1 This is a flowchart of the numerical simulation method.

[0037] Figure 2 This is a model diagram of the passive waste heat removal system on the secondary side. Detailed Implementation

[0038] The present invention will now be described in further detail with reference to the accompanying drawings and specific embodiments.

[0039] like Figure 1 As shown, the present invention provides a numerical simulation calculation method for high-pressure steam condensation in pipelines, comprising the following steps: Step 1: Design a pipe model that meets the thermodynamic requirements of the passive waste heat removal system on the secondary side of the pressurized water reactor. A schematic diagram of the passive waste heat removal system on the secondary side of the pressurized water reactor is shown below. Figure 2 As shown. The C-type heat exchanger in the secondary passive waste heat removal system adopts a coaxial condenser design. Due to the high steam temperature and pressure at the inlet, conventional pipe materials are insufficient for long-term use. To meet the requirements for temperature resistance, pressure resistance, and heat transfer, the internal steam channel heat transfer tubes are made of Inconel 690 tubing with a diameter of 29 mm × 5 mm and a maximum pressure resistance of: Formula (1) The system operating pressure is 17.5 MPa, and the coefficient is taken as 6. The tensile strength of Inconel 690 at 500℃ is greater than 500 MPa. Calculations show that the maximum pressure that the pipeline can withstand at 500℃ is greater than 20 MPa, which is higher than the system's maximum operating pressure of 17.5 MPa. Therefore, the pipeline wall thickness design meets the pressure requirements of the experiment.

[0040] The maximum pressure at the steam inlet is 17.5 MPa, the maximum flow velocity is 6 m / s, and the maximum superheat is 200 K. Therefore, the maximum volumetric flow rate is 6 × (0.019 / 2). 2 π = 0.0017012 m 3 The maximum mass flow rate is 0.0017012 × 51.347 = 0.08735 kg / s. The minimum heat transfer power required to ensure that all steam is converted into liquid phase is 0.08735 × (3436.8 - 1710.8) = 150.767 kW, of which the power for cooling superheated steam is 79.253 kW and the power for condensing saturated steam is 71.514 kW. A conservative estimate of the condensation heat transfer coefficient is 10 kW / (m²). 2 If the wall temperature remains at its maximum value (·K), then the required heat transfer tube length for the condensation section is 71.514 / (10×(627.82-553.15)×0.019π)=1.6045 m. The Reynolds number for the steam flow is... This exceeds the applicability of the Dittus-Boelter formula; therefore, the Gnielinski formula is used to calculate the Nusselt number for steam cooling heat transfer: Formula (2) In the formula, =0.0126576.

[0041] achievable f =0.0126576, Nu=1934, heat transfer coefficient is 16.174 kW / (m 2 The required length of the heat transfer tube for the cooling section is 79.253 / (16.174×(627.82-553.15)×0.019π)=1.0993 m.

[0042] If only heat exchange between steam and the heat transfer tube is considered, a 3-m heat transfer tube is sufficient to meet the heat transfer requirements. However, in actual experiments, it is also necessary to consider whether the heat transfer tube can quickly transfer heat to the cooling water. The heat transfer tube is made of Inconel 690 alloy, which has excellent corrosion resistance and oxidation resistance, good creep resistance, and excellent fatigue life. The maximum temperature of the heat transfer tube does not exceed 280 ℃, and the minimum temperature is room temperature. An average temperature of 150 ℃ is taken as the qualitative temperature, and the thermal conductivity is obtained by interpolation as 11.65 W / (m·K). The flow rate of the cooling water is set at 1 m / s based on the supply capacity of the experimental equipment. The provisional qualitative temperature is 40 ℃, and the corresponding mass flow rate is... 0.9226 kg / s. The cooling water temperature rise is 150.767 / (0.9226×4.182) = 39.092 ℃, therefore a qualitative temperature of 40 ℃ is reasonable. The Reynolds number of the cooling water is... 24316, of which D hydraulic diameter 0.016 m. The Reynolds number falls within the applicable range of the Dittus-Boelter formula, and its application in calculating the Nusselt number of the cooling water is... 133.3. The heat transfer coefficient between the cooling water and the outer wall of the heat transfer tube is... 5257.57 W / (m 2 ·K).

[0043] According to the heat transfer equation for the heat transfer process in a loop: Formula (3) Or written as Formula (4) The average temperature of the inner and outer walls of the heat transfer tube is difficult to determine. Adding the above three equations together and eliminating the others yields the result. t f1 The steam temperature is taken as 627.82 K, which is the saturation temperature. t f2 The cooling water temperature is taken as 313.15K from the qualitative temperature mentioned above; Φ is the heat flow rate. d 1.d 2 represents the inner and outer diameters of the heat transfer tube, respectively; h 1. h 2 represents the heat transfer coefficients of steam inside the heat transfer tube and cooling water outside the heat transfer tube, respectively. h The heat transfer coefficients of the steam cooling and condensation sections were obtained by weighted averaging. 12510 W / (m 2 ·K); l The calculated pipe length is 4.4098 m, but after retaining a certain margin, it is finally set at 5 m.

[0044] The external cooling jacket is made of 316L tubing. The gap between the external jacket and the heat transfer tubes cannot be too small, otherwise blockage is likely. This places extremely high demands on the straightness and installation accuracy of the pipes, resulting in a large pressure drop. Conversely, the gap cannot be too large either, otherwise the flow velocity will be too low, leading to decreased heat exchange efficiency and potentially requiring larger jacket sizes and more space, thus reducing economic efficiency. An 8 mm gap ensures good flow, acceptable pressure drop, and good heat exchange performance; therefore, the pipe diameter is 55 mm × 5 mm, and the length is 5000 mm.

[0045] Step 2: Based on the pipe model dimensions, create a 3D geometric model using SpaceClaim software. First, draw the projected shape of the steam flow domain on the planar sketch, then drag it to the appropriate length. Next, create the heat transfer pipe domain and the cooling water flow domain in sequence. It is important to note that when dragging the heat transfer pipe domain and the cooling water flow domain, the dragging method should be set to "non-merge" to correctly separate the three domains.

[0046] Step 3: Using ICEM software, divide the 3D geometric model into three blocks, corresponding to the steam flow domain, heat transfer pipe domain, and cooling water flow domain, respectively. Then, perform O-Block segmentation on each block. The middle sections of the heat transfer pipe domain and cooling water flow domain are hollow blocks; these middle blocks should be deleted. Then, map the vertices of the blocks to points on the corresponding domain edges, and map the outer and inner edges to the curves of the corresponding domains. Edit the parameters of each edge, including the number of vertices and the spacing and extension ratio of the boundary layers.

[0047] The number of vertices on an edge directly affects the mesh size and computational accuracy. If the mesh is too coarse, the gradients of physical quantities may not be accurately captured, resulting in significant discretization errors and impacting simulation accuracy. While excessive mesh refinement can improve accuracy, it significantly increases computational resource consumption and may even introduce numerical errors, reducing computational stability. By progressively refining the mesh and comparing the changes in key physical quantities, mesh independence can be considered achieved when these changes tend to stabilize.

[0048] Because the normal velocity and temperature exhibit a very large gradient near the wall, within a very small wall-normal distance, the velocity rises from rest relative to the wall to the mainstream velocity, and the fluid temperature rises from the temperature of undersaturated water to that of saturated steam or even superheated steam. Therefore, two methods are commonly used to calculate the flow field in this region: one is to use the wall function method; the other is to refine the mesh and use the wall model method to solve for the viscous sublayer. The choice between these two methods can be determined by the dimensionless wall distance. y + To reflect this.

[0049] Formula (5) In the formula, , τ w For wall shear force, y The normal distance to the wall. ρ The fluid density is given.

[0050] exist y + In the region where the velocity is less than 5, the velocity exhibits a nonlinear behavior; this region is commonly referred to as the viscous sublayer. y + In the region >60, velocity and distance show an almost linear trend. This region is the fully developed turbulence, also known as the logarithmic law region. The region between the two parts is often called the transition sublayer.

[0051] Using wall functions: Wall functions require the first layer mesh size to satisfy condition 30 < y + For values ​​less than 300, wall functions are unavailable when the size is too small, and cannot be used to solve for viscous sublayers when the size exceeds this range. High Reynolds number turbulence models (such as the standard k-ε model, Realizable k-ε model, RNG k-ε model, etc.) are typically used. Generally, wall functions can be used to solve for viscous sublayer data when they are not particularly important.

[0052] Solving for the viscous sublayer: To solve for the viscous sublayer, it is necessary to ensure that y + <1 (suggestion is to be close to 1). Because... y + The location of the first-layer mesh nodes is directly affected, therefore a very fine mesh is required when solving for viscous sublayers. For turbulence models, a low Reynolds number turbulence model (such as the k-ω model) should be selected. Generally, this method is used if the wall surface is crucial to the simulation results.

[0053] Since steam condensation and heat transfer almost entirely occur at the wall surface, the near-wall mesh is crucial for the simulation. Therefore, a method for solving the viscous sublayer is chosen to ensure...y + <1, divide the boundary layer mesh in the fluid domain on both sides of the heat transfer tube.

[0054] The mesh thickness of the first boundary layer can be calculated using the fluid's physical properties and flow state: 1) Calculate the Reynolds number. 2) Calculate the wall friction coefficient 3) Calculate the wall shear stress ;4) Calculation speed 5) Calculate the height of the first layer of mesh. .

[0055] Step 4: Select the appropriate multiphase flow model, turbulence model, and phase change model.

[0056] To better simulate the flow and heat transfer process of high-pressure steam condensing in a pipe, the Mixture model was used for multiphase flow, the SST k–ω model for turbulence, and the Lee model for phase change. The VOF model excels at capturing clear gas-liquid interfaces, but its computational grid requirements are extremely high, and its ability to handle phase changes and dispersed small droplets is not efficient enough. In the Eulerian model, strong interphase momentum exchange requires precise allocation of source terms to the equations of each phase; improper handling can easily lead to imbalances and divergences. The Mixture model can well simulate the flow pattern of a continuous liquid film phase with discrete droplet phases, showing improved stability compared to the VOF model and faster computation speed compared to the Eulerian model. The k–ω model exhibits high accuracy in the viscous sublayer and transition region, requires no complex wall functions, and can be directly integrated to the wall. The k–ε model is more robust in free shear flow far from the wall and in fully developed turbulent regions, and is insensitive to free-flow turbulence values. The SST k–ω model combines the advantages of both, exhibiting a k–ω model in the near-wall region (inner boundary layer) and transforming into a modified k–ε model in the outer boundary layer and free flow. The Lee model determines whether a phase transition occurs based on the temperature difference between the saturation temperature and the working fluid temperature, treating the temperature of the gas-liquid interface as the saturation temperature. When the interface temperature is lower than the liquid phase temperature, evaporation occurs; when the interface temperature is higher than the liquid phase temperature, condensation occurs. The Lee model overcomes the limitations of the phase interface and is the most commonly used phase transition model for condensation simulation, as well as the default phase transition model in Fluent.

[0057] Step 5: Define material properties, set calculation working conditions, phase interactions and boundary conditions. When calculating ocean conditions, a user-defined function (UDF) to control gravity changes also needs to be set.

[0058] High-pressure steam is set as the main phase, and high-pressure condensate, cooling water, and their gas phases as secondary phases. The density, specific heat, thermal conductivity, and dynamic viscosity of each phase at different temperatures are obtained by consulting the REFPROP fluid thermodynamics and transport properties database. Using the saturation temperature as a reference, the standard enthalpy of the liquid phase is set to 0, and the standard enthalpy of the gas phase is set to the same value as the latent heat of vaporization. The mass transfer mechanism from the high-pressure liquid phase to the high-pressure gas phase is set as evaporation-condensation, and the condensation relaxation coefficient is set to 10-500 based on the steam flow rate.

[0059] To ensure proper heat transfer, shadow surfaces must be established on the inner and outer walls of the heat transfer tubes. These shadow surfaces primarily handle the mesh interface between adjacent regions and are closely related to mesh continuity, data transfer, and computational accuracy. If Fluent cannot automatically generate shadow surfaces, two surfaces sharing a common node in different domains on the inner or outer wall must be merged into a new geometry using Boolean operations to automatically generate the shadow surfaces. Since the cooling water temperature is not significantly different from the ambient temperature, the outer casing is set as an adiabatic wall to reduce computational complexity. Velocity inlets are only suitable for incompressible flows, while mass inlets are only suitable for compressible flows. In waste heat removal systems, the steam inlet Mach number is generally no higher than 0.01, considered incompressible flow, therefore a velocity inlet is chosen. Turbulence parameters are set according to the hydraulic diameter and turbulence intensity; default settings or medium turbulence are sufficient. Pressure outlets are most commonly used, allowing pressure to develop freely at the outlet. Fluid recirculation settings are crucial for potential condensate recirculation at the condenser end; the recirculation direction should be set to Normal to Boundary, and low turbulence intensity is recommended for recirculation turbulence.

[0060] For both static tilting and rolling motions in marine conditions, a formulaic gravity setting is used to simulate the motion, and the varying gravitational acceleration can be directly input into Fluent. However, in swaying motion, the fluid's movement within the pipe occurs in a rotating, non-inertial reference frame, generating inertial forces such as the Coriolis force. Therefore, a UDF is needed to precisely control the motion in different directions and add inertial forces during swaying. First, the current time and grid coordinates are obtained. Then, the instantaneous rotation angle, angular velocity, and angular acceleration of the ship's bow roll motion are calculated based on the laws of simple harmonic motion. Next, based on these rotational motion parameters, the centripetal acceleration, tangential acceleration, and Coriolis acceleration generated by the fluid due to the rotation of the reference frame are calculated. Finally, these three inertial accelerations are multiplied by the fluid density and negatively evaluated to obtain the source term of the momentum equation, thus considering the influence of the ship's bow roll motion on the flow field in the CFD simulation.

[0061] Step 6: Set up spatial discretization methods for different physical quantities, and use the COUPLED method in Fluent to perform pressure-velocity coupled calculations.

[0062] The COUPLED method is chosen to handle the coupling relationship between velocity and pressure, which is particularly suitable for cases where variables in various conservation equations are interrelated, thus improving the stability and convergence of the solver during equation solving. During the discretization of the governing equations, the momentum, energy, and species transport terms are expressed in a second-order upwind scheme to improve numerical accuracy, while the pressure term interpolation uses a volume force weighted scheme to enhance simulation performance under natural convection or gravity-driven scenarios. Furthermore, a cell-based Green-Gaussian method is employed in the calculation of variable gradients to enhance the ability to capture the changing trends of variables in unstructured meshes.

[0063] Step 7: Set the flow Coulomb number and adjust the explicit relaxation factor and the sub-relaxation factor.

[0064] The flow Coulomb number is set to 1, and other relaxation factors are: pressure relaxation factor is set to 0.3, momentum relaxation factor is set to 0.2, energy relaxation factor is set to 0.5, volume fraction relaxation factor is set to 0.1, and turbulence relaxation factor is set to 0.5. The pressure, momentum, and energy relaxation factors can be adjusted appropriately according to the changes in the residual curve.

[0065] Step 8: Initialize the settings for temperature, pressure, and flow rate of the steam and cooling water domains, as well as the temperature of the heat transfer tube domain.

[0066] Initialize the temperature, pressure, and velocity of the steam flow domain to the same parameters as the inlet steam, and similarly initialize the temperature, pressure, and velocity of the cooling water flow domain to the same parameters as the inlet cooling water. The temperature of the heat transfer tube domain should not be too high, otherwise it will cause the cooling water to boil; nor should it be too low, otherwise the steam will condense instantaneously, which may lead to calculation divergence.

[0067] Step 9: Start the calculation and adjust the relaxation factor appropriately according to the residual fluctuation to stabilize the flow.

[0068] The core principles for setting the flow Coulomb number and other sub-relaxation factors are: starting small and gradually increasing, dynamic adjustment, and coordinating coupled solutions with adaptive time steps. Steam condensation involves a two-phase phase transition between gas and liquid, and the parameter gradient near the wall is extremely high, requiring high numerical stability and strict control of the Coulomb number and relaxation factor.

[0069] If the residual curve decreases slowly, the pressure, momentum, or energy relaxation factor can be increased by 0.1; if the curve fluctuates continuously, it needs to be decreased by 0.1; if the calculation diverges, it needs to be decreased by 0.2 or even more until the calculation converges.

[0070] Step 10: Export solution data. Based on the thermodynamic data of the nodes on the inner wall of the heat transfer tube and combined with the volume fraction cloud map, determine the flow state of the steam to ensure that the thermodynamic requirements of the passive waste heat removal system on the secondary side are met.

[0071] The above description is a further detailed explanation of the present invention in conjunction with specific preferred embodiments. However, it should not be considered that the specific embodiments of the present invention are limited to this. For those skilled in the art, several simple deductions or substitutions can be made without departing from the concept of the present invention, and all such deductions or substitutions should be considered to fall within the scope of patent protection determined by the submitted claims.

Claims

1. A numerical simulation calculation method for high-pressure steam condensation in pipelines, characterized in that: Includes the following steps: Step 1: Design a pipe model that meets the thermodynamic requirements of the passive waste heat removal system on the secondary side of the pressurized water reactor; Step 2: Based on the dimensions of the pipe model, use SpaceClaim software to create a 3D geometric model; Step 3: Use ICEM software to divide the 3D geometric model into three blocks, corresponding to the steam flow domain, heat transfer pipe domain and cooling water flow domain respectively, and then mesh each block. Step 4: Select the appropriate multiphase flow model, turbulence model, and phase change model; Step 5: Define material properties, set calculation working conditions, interphase interactions and boundary conditions. When calculating ocean conditions, a user-defined function (UDF) to control gravity changes also needs to be set. Step 6: Set up spatial discretization methods for different physical quantities, and use the COUPLED method in Fluent to perform pressure-velocity coupled calculations; Step 7: Set the flow Coulomb number and adjust the explicit relaxation factor and the sub-relaxation factor; Step 8: Initialize the settings for temperature, pressure, and flow rate of the steam and cooling water domains, as well as the temperature of the heat transfer tube domain; Step 9: Begin calculations and adjust the relaxation factor according to the residual fluctuations to stabilize the flow. Step 10: Export data. Based on the thermodynamic data of the nodes on the inner wall of the heat transfer tube and combined with the volume fraction cloud map, determine the flow state of the steam to ensure that the thermodynamic requirements of the passive waste heat removal system on the secondary side are met.

2. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 1, the C-type heat exchanger in the passive waste heat removal system on the secondary side adopts a shell-and-tube condenser design. The internal steam channel heat transfer tube is made of Inconel 690 nickel-based high-temperature alloy with a diameter of 29 mm × 5 mm and a length of 5000 mm. The external cooling shell is made of 316L stainless steel with a diameter of 55 mm × 5 mm and a length of 5000 mm.

3. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 3, each block needs to be divided into O-blocks when dividing the grid.

4. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 3, the mesh needs to be finer near the inner and outer pipe walls in the steam and cooling water flow areas to ensure... y + <1 and close to 1.

5. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 4, the multiphase flow model used is the Mixture model, the turbulence model is the SST k–ω model, and the phase change model is the Lee model.

6. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 5, high-pressure steam is set as the main phase, and high-pressure condensate, cooling water liquid and gas phases are the secondary phases; the saturation temperature is used as the reference temperature, the standard state enthalpy of the liquid phase is 0, and the standard state enthalpy of the gas phase is the same as the latent heat of vaporization; the mass transfer mechanism from the high-pressure condensate to the high-pressure steam gas phase in the interphase interaction is evaporation-condensation, and the condensation relaxation coefficient is 10-500 depending on the steam flow rate.

7. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 5, it is necessary to ensure that the shadow surfaces of the inner and outer walls of the heat transfer tube are established to achieve correct heat transfer. If Fluent cannot automatically generate shadow surfaces, the two surfaces of the inner or outer wall that share a common node in different domains need to be merged into a new geometry through Boolean operations to automatically generate shadow surfaces. The outer sleeve is set as an adiabatic wall to reduce the computational difficulty. The inlet is a velocity inlet, which is suitable for calculating incompressible flows. Turbulence parameters are set according to the hydraulic diameter and turbulence intensity. The outlet is a pressure outlet, which allows the pressure to develop freely at the outlet.

8. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 5, for the two types of motion in the ocean conditions, static tilting and undulating motion, a formulaic gravity setting is used to simulate the motion; while in the oscillating motion, the motion of the liquid in the pipe is the motion in a rotating non-inertial reference frame, which will generate inertial force. Therefore, UDF is needed to accurately control the motion in different directions and add inertial force in the oscillating motion.

9. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 6, the COUPLED method is used to handle the coupling relationship between velocity and pressure. During the discretization of the control equations, the momentum, energy, and species transport terms adopt the second-order upwind scheme to improve numerical accuracy, while the pressure term interpolation adopts the volume force weighting scheme in Fluent to improve the simulation effect under natural convection or gravity-driven scenarios. In the calculation of variable gradients, the element-based Green-Gaussian method is used to enhance the ability to capture the changing trends of variables in unstructured meshes.

10. The numerical simulation calculation method for high-pressure steam condensation in a pipeline according to claim 1, characterized in that: In step 7, the flow Coulomb number is set to 1, and the other relaxation factors are: pressure relaxation factor is set to 0.3, momentum relaxation factor is set to 0.2, energy relaxation factor is set to 0.5, volume fraction relaxation factor is set to 0.1, and turbulence relaxation factor is set to 0.

5. Subsequently, the pressure, momentum, and energy relaxation factors are adjusted according to the changes in the residual curve. If the curve decreases slowly, increase it by 0.1; if the curve fluctuates continuously, decrease it by 0.1.

Images