CFD-based liquefied natural gas recondenser structure optimization method and device

Abstract

This application discloses a CFD-based liquefied natural gas recondenser structural optimization method and device. The method establishes an initial model based on an assembly drawing and completes geometric preprocessing. The method extracts the fluid channel, segments and selects the computational domain, and locally densifies the key areas. The method uses a meshing tool to generate a polyhedron mesh and completes mesh independence verification. The polyhedron mesh is imported into the solver and the model is set. Boundary and wall conditions are set, and solver parameters are configured. The method sets the initial flow field using a hybrid initialization method, establishes flow monitoring windows and temperature monitoring windows, and adjusts the simulation until convergence. The method analyzes the temperature cloud map and flow vector map to adjust the baffle structure. The method adjusts the tower diameter and packing layer height based on the change curve of the physical quantity field of the packing layer to continuously improve the performance of the recondenser. The method solves the problem of how to deeply study the flow and heat transfer laws in the recondenser and obtain the flow field distribution characteristics, thereby improving the working performance of the recondenser.

Description

Technical Field

[0001] The present application relates to the field of computational fluid dynamics technology, and in particular to a CFD-based liquefied natural gas recondenser structure optimization method and device. Background Art

[0002] With the growing global demand for clean energy, liquefied natural gas (LNG), as an efficient and clean energy carrier, has attracted widespread attention and development in its reception, storage, and transportation technologies. LNG receiving stations unload LNG from LNG carriers into storage tanks, where it is then pressurized and regasified for external transport. This process generates a large amount of superheated boil-off gas (BOG). Recondensers are primarily used at LNG receiving stations. During this process, LNG is transported from production to consumption via pipelines without recondensing equipment. Due to various factors, including external environmental factors and equipment operation, some LNG inevitably absorbs heat and evaporates, forming superheated boil-off gas (BOG).

[0003] The generation of superheated boil-off gas (BOG) poses multiple challenges to liquefied natural gas (LNG) storage and transportation systems. First, the accumulation of BOG increases pressure within the tanks, posing a potential threat to their structural safety and stability. Second, the discharge of BOG not only wastes valuable energy resources but also has potential environmental impacts. Furthermore, the management and treatment of BOG increases the complexity and operating costs of storage and transportation systems.

[0004] However, the design and optimization of recondensers currently face numerous technical challenges. Recondensers are large in size, have complex internal geometries, and include multiple internal components, the synergistic interaction of which significantly influences the condensation effect. Furthermore, the complex cross-scale two-phase flow, heat, and mass transfer processes involved within the recondenser are highly nonlinear and inter-coupled, posing significant challenges to both theoretical analysis and numerical simulation. Currently, no macroscopic numerical simulations of recondensers have been conducted.

[0005] Therefore, how to deeply study the flow and heat transfer laws in the recondenser and obtain the flow field distribution characteristics has become a problem to be solved in order to optimize the structure of the recondenser. Summary of the Invention

[0006] In the embodiment of the present application, by providing a CFD-based liquefied natural gas recondenser structure optimization method, the problem of how to deeply study the flow and heat transfer laws in the recondenser and obtain the flow field distribution characteristics is solved, thereby improving the working performance of the recondenser.

[0007] In the first aspect, the embodiment of the present application provides a CFD-based liquefied natural gas recondenser structure optimization method, which includes: establishing an initial model and completing geometric preprocessing according to the assembly drawing of the liquefied natural gas recondenser; using preprocessing software to extract the internal fluid channel of the initial model, and deleting the solid wall part, dividing the fluid domain along the symmetry plane, selecting half of the flow channel as the calculation domain, and dividing the calculation domain into an upper area, a packing layer area and a lower area; creating a locally encrypted geometry for the key area, generating an intermediate model, importing the intermediate model into a meshing tool, generating a polyhedron mesh, and performing mesh independence verification, determining the polyhedron mesh size, and generating a final model; wherein the key area is the baffle, gas-liquid distribution plate and Liquid distribution pipe; import the polyhedron mesh into the solver and perform model settings; wherein, the model settings include the configuration of the multiphase flow model, turbulence model and porous medium model and the input of physical parameters; set boundary conditions and wall conditions, and configure the solver parameters; set the initial flow field through the hybrid initialization method, establish a flow monitoring window and a temperature monitoring window to monitor the calculation convergence, adjust the transient time step and run the simulation until convergence is reached; analyze the condensation heat transfer process through the temperature cloud map, and identify the flow field distribution law through the flow vector diagram; calculate the uniformity of gas-liquid distribution, and adjust the baffle structure; analyze the curve of the physical quantity field changing along the height of the packing layer area, adjust the tower diameter and the height of the packing layer area, and iteratively improve the performance of the liquefied natural gas recondenser.

[0008] In one possible implementation, the calculation domain is divided into an upper region, a packing layer, and a lower region, including: the upper region is the portion from the gas-liquid inlet to the gas-liquid distribution plate outlet; the packing layer region is the region filled with Raschig ring random packing; and the lower region is the portion from the packing layer region outlet to the liquefied natural gas recondenser outlet.

[0009] In a possible implementation, the polyhedral mesh is generated by using a boundary octree interpolation encryption method to perform local encryption to generate the polyhedral mesh.

[0010] In one possible implementation, the polyhedral mesh is imported into the solver, and the model is set up, including: selecting the VOF multiphase flow model to calculate the two-phase flow process of liquefied natural gas and gaseous boil-off gas; wherein the liquefied natural gas is the main phase and the gaseous boil-off gas is the secondary phase; adopting the Lee evaporation-condensation model to handle the interphase condensation mass transfer process; selecting the renormalization group turbulence model as the turbulence model, and using the standard wall function; adopting the porous medium model to replace the packing layer region, using the simulation experiment to calibrate the empirical parameters of the two-phase corrected Eugen equation, and calculating the viscous loss coefficient and inertial loss coefficient in the porous medium model through the two-phase corrected Eugen equation; setting the natural gas component in REFPROF, using the KW3 model to fit the mixture physical properties, obtaining the variation law of the mixture physical properties with temperature, and obtaining the temperature correlation equation; wherein the mixture physical properties include density, viscosity, thermal conductivity and specific heat capacity; converting the temperature correlation equation into a piecewise polynomial form and inputting it into the solver.

[0011] In one possible implementation, the setting of boundary conditions and wall conditions includes: setting the gas-liquid phase inlet as a mass flow inlet, the gas-liquid phase outlet as a pressure outlet, defining turbulence intensity and hydraulic diameter; and setting the wall as an adiabatic and no-slip boundary condition.

[0012] In one possible implementation, the configuration of solver parameters includes: selecting a pressure-based solver for steady-state calculations and setting the gravity direction; using a coupling algorithm combined with a pseudo-transient method to enhance calculation convergence; selecting a second-order upwind scheme as the discretization method for the momentum equation and the energy equation, and first using a first-order upwind scheme for preliminary calculations of the turbulent kinetic energy and turbulent dissipation rate equations, and then switching to a second-order upwind scheme after the residual curve stabilizes to improve accuracy.

[0013] In one possible implementation, the initial flow field is set by a hybrid initialization method, a flow monitoring window and a temperature monitoring window are established to monitor the convergence of the calculation, the transient time step is adjusted and the simulation is run until convergence is reached, including: establishing a flow monitoring window, the horizontal axis is used to record the number of iteration steps, and the vertical axis is used to display the changes in the net flow rate of the inlet and outlet; establishing a temperature monitoring window, the horizontal axis is used to record the number of iteration steps, and the vertical axis is used to display the average temperature of the outlet section; setting the pseudo-transient time step and the total number of iteration steps, and starting the simulation calculation; according to the monitoring results of the flow monitoring window and the temperature monitoring window, if the flow and temperature fluctuate near the expected true value, reducing the pseudo-transient time step to a preset threshold to improve the calculation accuracy; continuously observing the monitoring window until the convergence standard is met when the net flow rate of the inlet and outlet is close to 0 and the outlet temperature is stable, and the simulation calculation is ended.

[0014] In one possible implementation, the condensation heat transfer process is analyzed by temperature cloud maps, and the flow field distribution pattern is identified by flow vector maps, including: making a longitudinal cross-sectional view perpendicular to the flow direction of the liquid phase inlet, observing the temperature distribution cloud map in the upper area, and clarifying the heat transfer situation and temperature gradient; setting a flow vector map on the axial symmetry surface of the final model to intuitively display the flow conditions of the gas phase and liquid phase, and observing vortices, backflows or uneven flow phenomena in the flow pattern.

[0015] In a possible implementation, the calculation of the gas-liquid distribution uniformity and the adjustment of the baffle structure include: making a cross section near the outlet of the gas-liquid distribution plate, establishing an outlet velocity cloud map, and calculating the uniformity of the gas-liquid distribution plate according to the formula Calculate the uniformity of gas-liquid distribution; where v i is the flow velocity of each outlet channel of the gas-liquid distribution plate, is the average flow velocity at the outlet of the distribution plate, and U is the distribution uniformity of gas and liquid; according to the calculated distribution uniformity of gas and liquid, the structure of the gas phase baffle and the liquid distribution pipe is adjusted; wherein, the adjustment method is to increase the baffle area or increase the distance between the baffle and the inlet and adjust the spacing between the liquid distribution pipe channels.

[0016] In the second aspect, an embodiment of the present application provides a CFD-based liquefied natural gas recondenser structure optimization device, which includes: a geometric modeling module, which is used to establish an initial model and complete geometric pre-processing according to the assembly drawing of the liquefied natural gas recondenser; using pre-processing software to extract the internal fluid channel of the initial model, delete the solid wall part, divide the fluid domain along the symmetry plane, select half of the flow channel as the calculation domain, and divide the calculation domain into an upper area, a packing layer area and a lower area; a meshing module, which is used to create a locally encrypted geometric body for the key area, generate an intermediate model, import the intermediate model into a meshing tool, generate a polyhedron mesh, perform mesh independence verification, determine the polyhedron mesh size, and generate a final model; wherein, the key area is the baffle, gas-liquid distribution plate and liquid Distribution pipe; model setting and calculation module, used to import polyhedral mesh into the solver and perform model setting; wherein, the model setting includes the configuration of multiphase flow model, turbulence model and porous medium model and the input of physical parameters; setting boundary conditions and wall conditions, and configuring solver parameters; setting the initial flow field through the hybrid initialization method, establishing the flow monitoring window and the temperature monitoring window to monitor the calculation convergence, adjusting the transient time step and running the simulation until convergence is reached; analysis and optimization module, used to analyze the condensation heat transfer process through the temperature cloud map, and identify the flow field distribution law through the flow vector map; calculate the distribution uniformity of gas and liquid, and adjust the baffle structure; analyze the curve of the physical quantity field changing along the height of the packing layer area, adjust the tower diameter and the height of the packing layer area, and iteratively improve the performance of the liquefied natural gas recondenser.

[0017] One or more technical solutions provided in the embodiments of this application have at least the following technical effects:

[0018] The embodiment of the present application provides a CFD-based liquefied natural gas recondenser structure optimization method. By accurately extracting the internal fluid channels, the high fidelity of the model is ensured, and the errors caused by model simplification are effectively reduced. A polyhedral mesh is generated and locally encrypted in key areas, which not only improves the mesh quality but also significantly improves the calculation accuracy. At the same time, the optimal mesh size is determined after mesh independence verification, ensuring the efficient use of computing resources. Through the setting of the multiphase flow model, the selection of the appropriate turbulence model, the configuration of the porous medium model and the input of accurate physical parameters, a high-precision simulation of the complex flow and heat transfer process inside the liquefied natural gas recondenser is achieved, providing a reliable basis for the optimization design. The initial flow field is set using a hybrid initialization method, and the flow and temperature monitoring windows are combined to monitor the calculation convergence in real time. By adjusting the pseudo-transient time step, the simulation process is effectively accelerated, ensuring that the convergence standard is reached in a relatively short time. The gas-liquid distribution law is intuitively obtained through the temperature cloud map, and the vortex problem area in the flow field is accurately identified in combination with the flow vector map, providing an intuitive basis for structural optimization. Furthermore, based on the calculation results of the uniformity of gas-liquid distribution, the baffle structure was adjusted in a targeted manner, which effectively improved the gas-liquid distribution and increased the heat transfer efficiency. The curve of the physical quantity field along the height change of the packing layer area was deeply analyzed to achieve the optimization of the design of the gas-liquid flow operating parameters, and the rationality of the tower diameter and the height of the packing layer area was scientifically evaluated. The overall performance of the liquefied natural gas recondenser was continuously improved through iterative optimization to ensure the safe operation of the liquefied natural gas recondensation process system. This application can intuitively obtain the flow and heat transfer laws in the recondenser, obtain the flow field distribution characteristics, and provide effective guidance for the optimization design of the recondenser structure, which is conducive to improving the working performance of the recondenser. BRIEF DESCRIPTION OF THE DRAWINGS

[0019] In order to more clearly illustrate the embodiments of the present application or the technical solutions in the prior art, the following briefly introduces the drawings required for use in the embodiments of the present application or the description of the prior art. Obviously, the drawings described below are some embodiments of the present application. For ordinary technicians in this field, other drawings can be obtained based on these drawings without paying any creative work.

[0020] Figure 1 A flow chart of a CFD-based liquefied natural gas recondenser structure optimization method provided in an embodiment of the present application;

[0021] Figure 2 A specific flow chart for importing a polyhedral mesh into a solver and performing model settings provided in an embodiment of the present application;

[0022] Figure 3 A specific flow chart for configuring solver parameters provided in an embodiment of the present application;

[0023] Figure 4 A specific flow chart for setting the initial flow field using a hybrid initialization method, establishing a flow monitoring window and a temperature monitoring window to monitor computational convergence, adjusting the transient time step, and running the simulation until convergence is achieved, provided in an embodiment of the present application;

[0024] Figure 5 A schematic diagram of the structure of a liquefied natural gas recondenser provided in an embodiment of the present application;

[0025] Figure 6 A temperature cloud map of the upper area provided in an embodiment of the present application;

[0026] Figure 7 A flow vector diagram on the axial symmetry plane of the final model provided in an embodiment of the present application;

[0027] Figure 8 A schematic diagram of the relationship between flow rate and packing layer area height under different parameters provided in the embodiments of the present application;

[0028] Figure 9 A schematic diagram of the relationship between the packing layer area height and pressure under different parameters provided in the embodiments of the present application;

[0029] Figure 10 A schematic diagram of the relationship between the packing layer area height and the gas phase condensation rate under different parameters provided in the embodiments of the present application;

[0030] Figure 11 A schematic diagram of a CFD-based liquefied natural gas recondenser structure optimization device provided in an embodiment of the present application;

[0031] Figure 12 Schematic diagram of a CFD-based liquefied natural gas recondenser structure optimization server provided in an embodiment of the present application. DETAILED DESCRIPTION

[0032] The following will be combined with the accompanying drawings in the embodiments of this application to clearly and completely describe the technical solutions in the embodiments of this application. Obviously, the described embodiments are part of the embodiments of this application, not all of the embodiments. Based on the embodiments in this application, all other embodiments obtained by ordinary technicians in this field without making creative efforts are within the scope of protection of this application.

[0033] The following description of some of the technologies involved in the embodiments of this application is provided to facilitate understanding and should be considered merely exemplary. Therefore, those skilled in the art will recognize that various changes and modifications may be made to the embodiments described herein without departing from the scope and spirit of this application. Similarly, for the sake of clarity and conciseness, some descriptions of well-known functions and structures are omitted from the following description.

[0034] The embodiment of the present application provides a CFD-based liquefied natural gas recondenser structure optimization method, such as Figure 1 As shown, the method includes steps S101 to S109. Figure 1 This is only an execution sequence shown in the embodiment of the present application, and does not represent the only execution sequence of the CFD-based liquefied natural gas recondenser structure optimization method. If the final result can be achieved, Figure 1 The steps shown may be performed in parallel or reversed.

[0035] S101: Based on the assembly drawing of the liquefied natural gas recondenser, establish the initial model and complete the geometric preprocessing.

[0036] Specifically, it is necessary to obtain detailed assembly drawings of the liquefied natural gas recondenser. These drawings should include the size, position relationship and connection method of all components. Use 3D modeling software to create an initial model based on the assembly drawing. During the modeling process, follow the instructions of the assembly drawing to add key components such as the cylinder, upper and lower heads (elliptical heads), gas-liquid distribution plate, liquid distribution pipe, etc. one by one. Pay attention to maintaining the relative position and connection relationship between the components and the assembly Figure 1 Identify and remove structures in the model that are not related to the internal fluid flow and heat transfer process, such as mounting holes, connection structures (such as flanges, bolts, etc.), measurement structures (such as thermometer sleeves), fixed structures (such as brackets, lifting lugs), etc. The removal of these structures helps to simplify the model, reduce the amount of calculation, and improve the accuracy of the simulation. Carefully check all fillet parts in the model, which are usually used to reduce stress concentration and increase structural strength in actual manufacturing. In the modeling software, use the fillet tool to smooth all fillets in the model, that is, smooth fillets. The smoothed fillets can reduce mesh distortion in numerical simulations and improve calculation stability and accuracy.

[0037] S102: Use pre-processing software to extract the internal fluid channel of the initial model, delete the solid wall part, divide the fluid domain along the symmetry plane, select half of the flow channel as the calculation domain, and divide the calculation domain into the upper area, the packing layer area and the lower area.

[0038] Figure 5 The schematic diagram of the structure of the liquefied natural gas recondenser provided in the embodiment of the present application is as follows: Figure 5 As shown, Figure 5(a) is the gas-liquid distribution plate, Figure 5 (b) is the liquid distribution pipe. Figure 5 (c) in the figure is the Raschig ring random packing area.

[0039] Specifically, the initial model is imported into the pre-processing software, and the pre-processing software used in this application is SpaceClaim. The volume extraction function in SpaceClaim is used to extract the internal fluid channels from the initial model. Since the recondenser is symmetrical, the fluid domain can be divided into two identical regions along its axial symmetry plane. In SpaceClaim, by selecting the symmetry plane and performing the split operation, the fluid domain is divided into two, and half of the flow channel is selected as the calculation domain as the calculation domain for subsequent numerical simulation. The calculation domain is divided into an upper area, a packing layer area, and a lower area. The upper area is the part from the gas-liquid inlet to the gas-liquid distribution plate outlet, and this area mainly undergoes the gas mixing and distribution process. The packing layer area is the area filled with Raschig ring random packing, within the height range of 200mm to 3500mm below the gas-liquid distribution plate, and this area is the core area of ​​the condensation process. The lower area is the part from the packing layer area outlet to the liquefied natural gas recondenser outlet, and this area involves the collection and discharge process of the condensed liquid. After completing the division of the computational domain, each boundary surface needs to be named to facilitate the subsequent setting of boundary conditions and result analysis. This usually includes key boundaries such as inlets and outlets, walls, and symmetry surfaces.

[0040] S103: Create locally refined geometry for key areas, generate an intermediate model, import the intermediate model into the meshing tool, generate a polyhedral mesh, perform mesh independence verification, determine the polyhedral mesh size, and generate the final model. The key areas are the baffles, gas-liquid distribution plate, and liquid distribution pipes.

[0041] Specifically, it is necessary to identify and determine the key areas that need to be encrypted, namely baffles, gas-liquid distribution plates and liquid distribution pipes. These areas require finer grids to accurately capture flow details due to their complex structures or important fluid dynamic characteristics. Create locally encrypted geometries for the key areas and generate intermediate models, which tightly cover the above-mentioned key areas. Ensure that the relationship between these encrypted geometries and the fluid domain is set to not merge so that they can be processed independently during the meshing process. Save the initial model containing the locally encrypted geometries as an intermediate model. The intermediate model contains the definitions of the encrypted area and the non-encrypted area. Import the intermediate model into the meshing tool. The meshing tool used in this application is Fluent Meshing, which is specifically used to generate high-quality CFD (computational fluid dynamics) grids. In Fluent Meshing, the boundary octree interpolation encryption method (BOI) is used for local encryption to generate polyhedral grids for the key areas. The BOI method can automatically adjust the grid density based on the geometric shape of the boundary, thereby achieving local encryption while maintaining the grid quality. Set the maximum grid size to 5mm for the encrypted area to ensure that the grids in these areas are fine enough. Set the mesh size range for the global region to 9-20 mm. Apply these settings and generate a polyhedral mesh in Fluent Meshing. Polyhedral meshes typically have good mesh quality and a low mesh count, making them suitable for CFD simulations of complex geometries. Determine mesh independence by gradually refining the mesh, for example by trying smaller mesh sizes in the refined region and then in the global region, and comparing the results (e.g., velocity and temperature fields) at different mesh densities. Determine the appropriate mesh size based on the mesh independence verification results.

[0042] S104: Import the polyhedral mesh into the solver and perform model settings, which include configuring the multiphase flow model, turbulence model, and porous media model, as well as inputting physical property parameters.

[0043] Figure 2 The specific flow chart of importing the polyhedral mesh into the solver and setting up the model provided in the embodiment of the present application is as follows: Figure 2 As shown, it includes steps S201 to S206.

[0044] S201: Selecting the VOF multiphase flow model to calculate the two-phase flow process of liquefied natural gas and gaseous boil-off gas, wherein the liquefied natural gas is the primary phase and the gaseous boil-off gas is the secondary phase.

[0045] S202: The Lee evaporation-condensation model is used to process the interphase condensation mass transfer process.

[0046] Specifically, the VOF multiphase flow model is a numerical method for simulating the interface between two or more immiscible fluids. When simulating the changes in the phase interface between liquefied natural gas (LNG) and gaseous boil-off gas (BOG), the VOF model accurately describes their spatial distribution and dynamic changes by tracking the volume fractions of liquefied natural gas and gaseous boil-off gas. Specifically, liquefied natural gas is set as the main phase, and gaseous boil-off gas is set as the secondary phase. During the simulation process, the VOF model continuously updates the volume fraction in each grid cell according to the flow and interaction of the fluid, thereby accurately capturing the phase interface. In order to more realistically simulate the interaction between liquefied natural gas and gaseous boil-off gas, this application also combines the Lee evaporation-condensation model to deal with the mass transfer between phases. The Lee evaporation-condensation model is an empirical model based on experimental data, which is used to describe the rate of mass transfer of fluids during evaporation and condensation. In this application, the evaporation-condensation coefficient is set to 12.

[0047] As the simulation progresses, the VOF multiphase flow model continuously updates the volume fractions within the grid cells based on factors such as the fluid's flow characteristics and boundary conditions. As the liquefied natural gas (LNG) evaporates, its volume fraction decreases, while the volume fraction of the vapor gas increases accordingly. Conversely, as the vapor gas condenses, its volume fraction decreases, while the volume fraction of the LNG increases. This approach simulates the interface changes between the LNG and vapor gas, as well as the mass transfer between them.

[0048] S203: The turbulence model uses the renormalization group turbulence model and the standard wall function.

[0049] Specifically, the renormalized group turbulence model is the RNG k-epsilon model. When simulating turbulent flows, especially those involving flows near walls, it is necessary to combine it with standard wall functions to account for the flow characteristics near walls. Standard wall functions are semi-empirical models used to describe the velocity distribution and turbulence characteristics near walls. By combining the RNG k-epsilon model with standard wall functions, turbulent flows near walls can be simulated more accurately.

[0050] S204: The packing layer area is equivalently replaced by a porous medium model, and the empirical parameters of the two-phase corrected Eugen equation are calibrated using a modeling experiment. The viscous loss coefficient and the inertial loss coefficient in the porous medium model are calculated using the two-phase corrected Eugen equation.

[0051] Specifically, during the simulation, the complex structure of the packing layer region made it difficult to establish a specific geometric model. However, the random packing layer region of the Raschig ring packing can be equivalent to an isotropic porous medium. Therefore, a porous medium model was used to accurately describe the flow behavior of the fluid through the random packing. To calculate the viscous and inertial loss coefficients for the porous medium model, a two-phase modified Eugen equation was employed. This equation fully accounts for the characteristics of gas-liquid two-phase flow, resulting in calculation results that are closer to the actual physical process. The calculation of the viscous and inertial loss coefficients incorporates the characteristic parameters of the random packing, such as porosity, particle shape, and size distribution, which significantly influence the fluid flow resistance. By inputting these random packing characteristic parameters into the two-phase modified Eugen equation, the viscous and inertial loss coefficients applicable to the current simulation conditions can be obtained. The empirical parameters E1 and E2 of the Eugen equation are related to the geometric structure and distribution. To ensure the accuracy and reliability of the calculation results, a recondenser simulation experiment was conducted to calibrate the empirical parameters in the Eugen equation. In this application, the empirical parameters are E1 = 381.2 and E2 = 1.7. Applying the calibrated empirical parameters to the two-phase modified Eugen equation can further improve the calculation accuracy of the viscous loss coefficient and the inertial loss coefficient.

[0052] S205: Set the natural gas composition in REFPROF, use the KW3 model to fit the mixture's physical properties, and obtain the temperature-dependent variation of the mixture's physical properties, including density, viscosity, thermal conductivity, and specific heat capacity, to obtain a temperature correlation equation.

[0053] S206: Convert the temperature correlation equation into a piecewise polynomial form and input it into the solver.

[0054] Specifically, the natural gas composition settings in the REFPROF software are designed to accurately simulate the physical behavior of natural gas under different temperature conditions. To achieve this goal, the KW3 model (a model specifically designed for calculating the physical properties of mixtures) was used to obtain the comprehensive physical properties of these components. This model, through thermodynamic and fluid dynamics calculations, can predict various physical properties of mixtures at different temperatures. Specifically, the KW3 model was used to calculate the four key physical properties of the gas phase (BOG) and liquid phase (LNG) of the natural gas mixture, namely, the boil-off gas and liquefied natural gas, at different temperatures. These parameters include density, viscosity, thermal conductivity, and specific heat capacity. Polynomial fitting was used to describe the variations in the physical properties of natural gas within the recondenser operating temperature range (110K to 260K) in the form of piecewise polynomials or continuous functions. Polynomial fitting is a mathematical tool that constructs a polynomial function based on discrete points obtained from experimental data or theoretical calculations to approximate the continuous variation between these points. Compared to simple linear fitting, polynomial fitting can more accurately capture the nonlinear characteristics of the physical properties as they vary with temperature. During implementation, the numerical values ​​of natural gas physical properties, such as density, viscosity, thermal conductivity, and specific heat capacity at constant pressure, at different temperatures are first collected or calculated. Then, using mathematical software or programming tools, polynomial fitting is performed on these data to obtain a polynomial expression for each physical parameter as it varies with temperature. The coefficients and order of these polynomial expressions are adjusted based on the accuracy and complexity of the fitting to ensure that they accurately reflect the actual changing trends of the physical parameters.

[0055] As shown in Table 1, this temperature correlation allows for the rapid and accurate calculation of corresponding physical property values ​​for any given temperature. The resulting polynomial expressions are fed into the solver as input data for natural gas physical properties. During the simulation, the solver uses these polynomial expressions to calculate the corresponding physical property values ​​in real time based on the current temperature, thereby accurately simulating the flow and heat transfer of natural gas within the recondenser.

[0056] Table 1

[0057]

[0058] S105: Set boundary conditions and wall conditions, and configure solver parameters.

[0059] Set boundary and wall conditions, including: setting the gas and liquid phase inlets to mass flow inlets, the gas and liquid phase outlets to pressure outlets, and defining the turbulence intensity and hydraulic diameter. Set the walls to adiabatic and no-slip boundary conditions.

[0060] Figure 3The specific flow chart for configuring solver parameters provided in the embodiment of the present application is as follows: Figure 3 As shown, it includes steps S301 to S303.

[0061] S301: Select the pressure-based solver for steady-state calculation and set the gravity direction.

[0062] Specifically, in this application, the direction of gravity is set to the negative direction of the y-axis to ensure that the fluid dynamics behavior in the simulation is consistent with the actual situation.

[0063] S302: Adopting coupling algorithm combined with pseudo-transient method to enhance computational convergence.

[0064] Specifically, to more accurately solve the velocity and pressure coupling problem in fluid flow, a coupled algorithm (Coupled algorithm) is selected for solution. The Coupled algorithm can solve the momentum equation and the continuity equation simultaneously, which helps reduce the number of iterations and improve the convergence speed. At the same time, to further enhance convergence, the pseudo-transient method is enabled. The pseudo-transient method simulates transient effects by introducing a time term during the iteration process, which helps stabilize the solution process, especially in complex flows or with high turbulence intensity.

[0065] S303: The second-order upwind scheme is selected as the discretization method for the momentum equation and the energy equation. The first-order upwind scheme is used for preliminary calculation of the turbulent kinetic energy and turbulent dissipation rate equations. After the residual curve stabilizes, the second-order upwind scheme is used to improve the accuracy.

[0066] Specifically, the second-order upwind scheme was chosen as the discretization method for the momentum and energy equations. This high-order discretization method can more accurately capture fluctuations and changes in fluid flow, improving the accuracy of the solutions to the momentum and energy equations, but its convergence is poor. The turbulent kinetic energy and turbulent dissipation rate equations were initially calculated using the first-order upwind scheme. Although the first-order upwind scheme has lower accuracy, it has good computational stability and is suitable for initialization and rapid convergence. After convergence, the second-order upwind scheme is switched to improve accuracy.

[0067] S106: Setting the initial flow field through a hybrid initialization method, establishing a flow monitoring window and a temperature monitoring window to monitor the computational convergence, adjusting the transient time step, and running the simulation until convergence is achieved.

[0068] Figure 4 The embodiment of the present application provides a specific flow chart for setting the initial flow field by a hybrid initialization method, establishing a flow monitoring window and a temperature monitoring window to monitor the calculation convergence, adjusting the transient time step and running the simulation until convergence is achieved, as shown in FIG. Figure 4As shown, it includes steps S401 to S405.

[0069] S401: A flow monitoring window is established, where the horizontal axis is used to record the number of iteration steps, and the vertical axis is used to display the changes in the net flow rate of the inlet and outlet.

[0070] Specifically, the Flow Monitoring window is used to monitor the net flow rate between the inlet and outlet in real time. The horizontal axis of this window is set to the number of iterations, recording the progress of the simulation. The vertical axis displays the real-time value of the net flow rate between the inlet and outlet, helping users understand how the flow rate changes with the number of iterations.

[0071] S402: Establish a temperature monitoring window, where the horizontal axis is used to record the number of iteration steps, and the vertical axis is used to display the average temperature of the outlet section.

[0072] Specifically, the Temperature Monitoring window monitors the average temperature of the outlet section. Similar to the Flow Monitoring window, the horizontal axis of this window displays the number of iterations, while the vertical axis displays the real-time value of the average temperature of the outlet section, helping users determine whether the temperature has reached a stable state.

[0073] S403: Set the pseudo-transient time step and the total number of iteration steps, and start simulation calculation.

[0074] Specifically, before starting the simulation, it is necessary to set the pseudo-transient time step and the total number of iterations. The initial pseudo-transient time step of this application is set to 8, and the total number of iterations is set to 50,000 steps. Then, the simulation calculation is started to start the simulation of the fluid flow. Of course, the specific values ​​of the transient time step and the total number of iterations can be set to other values, and this application is not limited to the above values.

[0075] S404: Based on the monitoring results of the flow monitoring window and the temperature monitoring window, if the flow and temperature fluctuate around the expected true value, the pseudo-transient time step is reduced to a preset threshold to improve calculation accuracy.

[0076] Specifically, during the simulation process, the monitoring results of the flow monitoring window and the temperature monitoring window are checked regularly. If the flow and temperature are found to fluctuate near the expected true value, it indicates that the current calculation may be too rough or not stable enough, and the pseudo-transient time step needs to be adjusted. This application reduces the pseudo-transient time step to 0.1, that is, the preset threshold is 0.1, to improve the accuracy and stability of the calculation. Of course, the preset threshold can be set to other values, and this application is not limited to the above values.

[0077] S405: Continuously observe the monitoring window until the inlet and outlet net flow rates are close to 0 and the outlet temperature remains stable, reaching the convergence standard, and then end the simulation calculation.

[0078] Specifically, during the simulation, it's necessary to constantly monitor the real-time data in the flow monitoring window and the temperature monitoring window. The vertical axis of the flow monitoring window displays the change in the net inlet and outlet flow rate over the number of iterations, while the vertical axis of the temperature monitoring window displays the change in the average temperature of the outlet cross-section. The net inlet and outlet flow rate is an important indicator of the fluid flow between the inlet and outlet. When the simulation progresses to a certain point, if the net inlet and outlet flow rate gradually decreases and approaches zero, it indicates that the fluid flow in the system has reached equilibrium, with no significant net flow entering or leaving the system. In practice, a threshold can be set (such as the absolute value of the net flow rate being less than a small number). When the net inlet and outlet flow rates remain within this threshold for multiple consecutive iterations, the net flow rate is considered close to zero. The stability of the outlet temperature is another important criterion for determining whether the simulation has converged. When the system reaches a stable state, the average temperature of the outlet cross-section should remain at a relatively constant value, without significant fluctuations. To determine whether the outlet temperature is stable, observe the temperature curve in the temperature monitoring window. If the curve remains flat or has only slight fluctuations for a period of time, the outlet temperature is considered stable. When both the inlet and outlet net flow rates are close to zero and the outlet temperature remains stable, the simulation is considered to have reached convergence. At this point, further iterations of the simulation can be stopped and the current simulation results saved.

[0079] S107: Analyze the condensation heat transfer process through the temperature cloud diagram and identify the flow field distribution pattern through the flow vector diagram.

[0080] Analyze the condensation heat transfer process using temperature cloud maps, and identify the flow field distribution pattern using flow vector diagrams. This includes creating a longitudinal cross-section perpendicular to the liquid inlet flow direction and observing the temperature distribution cloud map in the upper region to clarify the heat transfer and temperature gradient. Set a flow vector diagram on the axially symmetric plane of the final model to visually display the flow of the gas and liquid phases and observe eddies, backflows, or uneven flow patterns.

[0081] Specifically, the steps for in-depth heat transfer analysis using temperature contours include creating a vertical cross-section perpendicular to the liquid inlet flow direction and observing the temperature distribution contours in the upper region. This step aims to gain key insights into the internal flow and heat transfer process and clarify the temperature gradient distribution pattern. Figure 6 The temperature cloud map of the upper area provided in the embodiment of this application is as follows: Figure 6 As shown in the figure, a clearly discernible interface is formed between the gas and liquid phases above the gas-liquid distribution plate in the recondenser. This phenomenon indicates that contact and mixing occur between the gas and liquid phases in this region. Due to the temperature difference, the condensation process is not significantly observed at this stage, indicating that heat transfer occurs primarily through sensible heat exchange.

[0082] A flow vector diagram is set on the axially symmetrical plane to intuitively display the flow behavior of the gas and liquid phases. The flow vector diagram can clearly identify eddies, backflows, or uneven flow in the flow field. These phenomena often lead to uneven gas-liquid distribution and indirectly cause poor condensation in the packing layer area. Figure 7 The flow vector diagram provided in the embodiment of the present application is set on the axial symmetric surface of the final model, such as Figure 7 As shown in the figure, the flow of the gas and liquid phases in the recondenser can be clearly seen. In the gas phase, the flow velocity in the near-wall area is significantly higher, and in the upper area, the gas phase flow forms a symmetrical vortex structure. This vortex phenomenon leads to poor uniformity in the gas phase distribution. To improve this situation, it is possible to consider increasing the distance between the gas baffle and the inlet to adjust the flow path of the gas phase and reduce the formation of vortices. Secondly, opening a hole in the center of the gas baffle is also an effective optimization method. It can promote the uniform distribution of the gas phase and reduce the occurrence of local excessive flow velocity and vortex phenomena. In contrast, the flow of the liquid phase in the tube appears relatively stable and more evenly distributed. This shows that the design of the liquid distribution tube is relatively reasonable and is conducive to the condensation heat transfer process in the packing layer area.

[0083] S108: Calculate the distribution uniformity of gas and liquid and adjust the baffle structure.

[0084] Calculate the uniformity of gas-liquid distribution and adjust the baffle structure, including: making a cross section near the outlet of the gas-liquid distribution plate, establishing an outlet velocity cloud map, and using the formula Calculate the uniformity of gas-liquid distribution. i is the flow velocity of each outlet channel of the gas-liquid distribution plate, is the average flow velocity at the distributor outlet, and U is the gas-liquid distribution uniformity. Based on the calculated gas-liquid distribution uniformity, the structure of the gas phase baffles and liquid distribution pipes is adjusted. Adjustments can be made by increasing the baffle area, increasing the distance between the baffles and the inlet, or adjusting the spacing between the channels in the liquid distribution pipes.

[0085] Specifically, the baffle structure is adjusted based on the calculated gas-liquid distribution uniformity. If the gas phase distribution is poor, the gas phase velocity near the wall can be reduced by increasing the baffle area or the distance between the baffle and the inlet, thereby improving the gas phase distribution uniformity. These adjustments help improve the fluid flow state within the recondenser and enhance heat exchange efficiency.

[0086] S109: Analyze the curve of the physical quantity field of the packing layer area along the height change, adjust the tower diameter and the height of the packing layer area, and iteratively improve the performance of the liquefied natural gas recondenser.

[0087] Specifically, by analyzing the curves of physical quantities (such as flow rate, pressure, and BOG condensation rate) that vary along the height of the packing layer, we gain a deeper understanding of the flow characteristics and heat transfer performance within the packing layer. By creating cross sections at different height intervals, such as every 300 mm, and monitoring the relevant physical quantities, we obtain detailed data support for evaluating the rationality of the recondenser design in the packing layer area.

[0088] Based on this data, we can further optimize the tower diameter and packing layer height. Increasing the tower diameter helps reduce fluid velocity and pressure drop, while increasing the packing layer height enhances heat transfer and improves condensation efficiency. Through multiple iterations of optimization and continuous comparison of performance under different structural parameters, we ultimately determined the optimal structural parameters for the LNG recondenser to maximize performance.

[0089] Figure 8 Schematic diagram of the relationship between flow rate and packing layer area height under different parameters provided in the embodiment of the present application, such as Figure 8 As shown in the figure, the horizontal axis represents the height of the packing layer in mm, and the vertical axis represents the flow rate in m / s. After entering the packing layer of the recondenser, the flow rate drops significantly due to the resistance of the packing layer. Within a certain height range of the packing layer, the flow rate gradually decreases and stabilizes, with an average flow rate of approximately 0.1 m / s. This reduction in flow rate helps enhance the interaction between the fluid and the packing, improving the heat and mass exchange performance of the recondenser.

[0090] Figure 9 Schematic diagram of the relationship between the packing layer area height and pressure under different parameters provided in the embodiment of the present application, such as Figure 9 As shown, the horizontal axis represents the height of the packing layer area, the unit is mm; the vertical axis represents the pressure, the unit is kPa. Figure 9 As can be seen, the pressure of the fluid increases approximately linearly in the packing area. This means that as the fluid penetrates deeper into the packing area, the pressure gradually increases in an approximately linear manner. This linear relationship indicates that the resistance or pressure increase exerted by the packing area on the fluid is uniform and predictable.

[0091] Figure 10 Schematic diagram of the relationship between the packing layer area height and the gas phase condensation rate under different parameters provided in the embodiment of the present application, such as Figure 10 As shown in the figure, the horizontal axis represents the height of the packing layer area, in mm; the vertical axis represents the condensation rate of gaseous boil-off gas (BOG). The condensation rate refers to the proportion of gaseous boil-off gas condensed into liquid in the packing layer area, which is an important indicator to measure the condensation effect. Figure 10It can be seen that the BOG condensation rate slows down as the tower diameter increases. At the same packing layer height, the growth rate of the BOG condensation rate gradually slows as the tower diameter increases. This is because the flow rate in the packing layer slows as the tower diameter increases, and these changes affect the heat and mass exchange efficiency between the fluid and the packing.

[0092] The embodiment of the present application also provides a CFD-based liquefied natural gas recondenser structure optimization device 1100, such as Figure 11 As shown, the device includes: a geometric modeling module 1101, a meshing module 1102, a model setting and calculation module 1103 and an analysis and optimization module 1104.

[0093] Geometric modeling module 1101 is used to build an initial model and perform geometric preprocessing based on the assembly drawing of the liquefied natural gas recondenser. Preprocessing software is used to extract the fluid channels within the initial model, delete the solid walls, and split the fluid domain along the symmetry plane. Half of the flow channel is selected as the computational domain, which is then divided into an upper region, a packing layer region, and a lower region.

[0094] Meshing module 1102 is used to create locally refined geometry for key areas, generate an intermediate model, import the intermediate model into the meshing tool, generate a polyhedral mesh, perform mesh independence verification, determine the polyhedral mesh size, and generate the final model. The key areas are the baffles, gas-liquid distribution plate, and liquid distribution pipes.

[0095] The model setup and calculation module 1103 is used to import the polyhedral mesh into the solver and perform model setup. This includes configuring the multiphase flow model, turbulence model, and porous media model, as well as inputting physical property parameters. Boundary and wall conditions are set, and solver parameters are configured. The initial flow field is set using a hybrid initialization method, flow monitoring windows and temperature monitoring windows are established to monitor computational convergence, and the transient time step is adjusted and the simulation is run until convergence is achieved.

[0096] The analysis and optimization module 1104 analyzes the condensation heat transfer process using temperature cloud maps and identifies flow field distribution patterns using flow vector diagrams. It calculates the uniformity of gas-liquid distribution and adjusts the baffle structure. It analyzes the curve of the physical field variation along the packing layer, adjusts the tower diameter and packing layer height, and iteratively improves the performance of the liquefied natural gas recondenser.

[0097] Some modules in the apparatus described herein may be described in the general context of computer-executable instructions executed by a computer, such as program modules. Generally, program modules include routines, programs, objects, components, data structures, classes, etc. that perform specific tasks or implement specific abstract data types. The present application may also be practiced in distributed computing environments where tasks are performed by remote processing devices connected via a communications network. In a distributed computing environment, program modules may be located in local and remote computer storage media, including storage devices.

[0098] The devices or modules described in the above application embodiments can be implemented by computer chips or physical devices, or by products with certain functions. For ease of description, the above devices are described separately by function in various modules. When implementing the embodiments of this application, the functions of each module can be implemented in the same or multiple software and / or hardware. Of course, a module that implements a certain function can also be implemented by combining multiple sub-modules or sub-units.

[0099] The methods, devices, or modules described in this application can be implemented in the form of computer-readable program code. The controller can be implemented in any appropriate manner. For example, the controller can take the form of a microprocessor or processor and a computer-readable medium storing computer-readable program code (such as software or firmware) that can be executed by the (micro)processor, logic gates, switches, application-specific integrated circuits (ASICs), programmable logic controllers, and embedded microcontrollers. Examples of controllers include, but are not limited to, the following microcontrollers: ARC 625D, Atmel AT91SAM, Microchip PIC18F26K20, and Silicone Labs C8051F320. The memory controller can also be implemented as part of the control logic of the memory. Those skilled in the art will also know that in addition to implementing the controller in the form of pure computer-readable program code, it is entirely possible to implement the same function of the controller in the form of logic gates, switches, application-specific integrated circuits, programmable logic controllers, and embedded microcontrollers by logically programming the method steps. Therefore, such a controller can be considered a hardware component, and the devices included therein for implementing various functions can also be considered as structures within the hardware component. Or even, the means for implementing various functions may be considered to be both a software module for implementing the method and a structure within a hardware component.

[0100] like Figure 12As shown, an embodiment of the present application further provides a CFD-based liquefied natural gas recondenser structure optimization server, including a memory 1201 and a processor 1202; the memory 1201 is used to store computer-executable instructions; the processor 1202 is used to execute computer-executable instructions to implement a CFD-based liquefied natural gas recondenser structure optimization method described above in the embodiment of the present application.

[0101] An embodiment of the present application further provides a computer-readable storage medium storing executable instructions. When a computer executes the executable instructions, the CFD-based liquefied natural gas recondenser structure optimization method described above in the embodiment of the present application can be implemented.

[0102] Through the description of the above implementation methods, it can be known that those skilled in the art can clearly understand that the present application can be implemented by means of software plus necessary hardware. Based on this understanding, the technical solution of the present application can be essentially or the part that contributes to the prior art can be embodied in the form of a software product, or it can be embodied in the implementation process of data migration. The computer software product can be stored in a storage medium, such as ROM / RAM, a magnetic disk, an optical disk, etc., and includes a number of instructions for enabling a computer device (which can be a personal computer, a mobile terminal, a server, or a network device, etc.) to execute the method described in the embodiment of the present application.

[0103] The various embodiments in this specification are described in a progressive manner. The same or similar parts between the various embodiments can be referred to in detail. Each embodiment focuses on the differences from other embodiments. All or part of this application can be used in many general or special computer system environments or configurations.

[0104] The above embodiments are only used to illustrate the technical solutions of the present application, rather than to limit the present application. Although the present application has been described in detail with reference to the aforementioned embodiments, a person of ordinary skill in the art should understand that the technical solutions described in the aforementioned embodiments can still be modified, or some or all of the technical features therein can be replaced by equivalents. However, these modifications or replacements do not cause the essence of the corresponding technical solutions to deviate from the scope of the technical solutions of the present application.

Claims

1. A CFD-based liquefied natural gas recondenser structure optimization method, characterized in that: include: According to the assembly drawing of the liquefied natural gas recondenser, the initial model was established and the geometric preprocessing was completed; The fluid channel inside the initial model is extracted using pre-processing software, and the solid wall portion is deleted, the fluid domain is divided along the symmetry plane, half of the flow channel is selected as the calculation domain, and the calculation domain is divided into an upper region, a packing layer region, and a lower region; Creating locally encrypted geometry for the critical areas, generating an intermediate model, importing the intermediate model into a meshing tool, generating a polyhedral mesh, performing mesh independence verification, determining the polyhedral mesh size, and generating a final model; wherein the critical areas are the baffles, gas-liquid distribution plate, and liquid distribution pipes; Importing the polyhedral mesh into the solver and performing model settings, wherein the model settings include configuring the multiphase flow model, turbulence model, and porous media model, and inputting physical property parameters; Set boundary conditions and wall conditions, and configure solver parameters; The initial flow field is set by a hybrid initialization method, flow monitoring windows and temperature monitoring windows are established to monitor the computational convergence, the transient time step is adjusted, and the simulation is run until convergence is achieved. Analyze the condensation heat transfer process through temperature cloud diagrams and identify the flow field distribution pattern through flow vector diagrams; Calculate the uniformity of gas-liquid distribution and adjust the baffle structure; By analyzing the curve of the physical quantity field changing along the height of the packing layer area, the tower diameter and the height of the packing layer area are adjusted to improve the performance of the liquefied natural gas recondenser in an iterative manner.

2. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The calculation domain is divided into an upper region, a packing layer and a lower region, comprising: The upper area is the part from the gas-liquid inlet to the gas-liquid distribution plate outlet; The packing layer area is the area filled with Raschig ring random packing; The lower area is the portion from the outlet of the packing layer area to the outlet of the liquefied natural gas recondenser.

3. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The polyhedral mesh generation method is: using a boundary octree interpolation encryption method to perform local encryption to generate the polyhedral mesh.

4. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The polyhedron mesh is imported into the solver and the model is set up, including: The VOF multiphase flow model is selected to calculate the two-phase flow process of liquefied natural gas and gaseous boil-off gas, where liquefied natural gas is the primary phase and gaseous boil-off gas is the secondary phase. The Lee evaporation-condensation model is used to deal with the interphase condensation mass transfer process; The turbulence model uses the renormalized group turbulence model and the standard wall function; The packing layer area is replaced by a porous medium model, and the empirical parameters of the two-phase modified Eugen equation are calibrated using simulation experiments. The viscous loss coefficient and inertial loss coefficient in the porous medium model are calculated using the two-phase modified Eugen equation. In REFPROF, natural gas components are set and the physical properties of the mixture are fitted using the KW3 model to obtain the variation pattern of the physical properties of the mixture with temperature, thereby obtaining a temperature correlation equation. The physical properties of the mixture include density, viscosity, thermal conductivity, and specific heat capacity. The temperature correlation equation is converted into a piecewise polynomial form and input into the solver.

5. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The setting of boundary conditions and wall conditions includes: Set the gas-liquid phase inlet as the mass flow inlet, the gas-liquid phase outlet as the pressure outlet, and define the turbulence intensity and hydraulic diameter; The walls are set to adiabatic and no-slip boundary conditions.

6. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The configuration solver parameters include: Select the pressure-based solver for steady-state calculations and set the gravity direction; The coupling algorithm is combined with the pseudo-transient method to enhance the computational convergence; The second-order upwind scheme is selected as the discretization method for the momentum equation and the energy equation. The turbulent kinetic energy and turbulent dissipation rate equations are initially calculated using the first-order upwind scheme. After the residual curve stabilizes, the second-order upwind scheme is used to improve the accuracy.

7. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The hybrid initialization method is used to set the initial flow field, establish a flow monitoring window and a temperature monitoring window to monitor the convergence of the calculation, adjust the transient time step and run the simulation until convergence is achieved, including: Establish a flow monitoring window, with the horizontal axis used to record the number of iteration steps and the vertical axis used to display the changes in the net flow rate of imports and exports; Establish a temperature monitoring window, with the horizontal axis used to record the number of iteration steps and the vertical axis used to display the average temperature of the outlet section; Set the pseudo-transient time step and the total number of iterations, and start the simulation calculation; Based on the monitoring results of the flow monitoring window and the temperature monitoring window, if the flow and temperature fluctuate around the expected true value, the pseudo-transient time step is reduced to the preset threshold to improve the calculation accuracy; Continue to observe the monitoring window until the net flow rate of inlet and outlet approaches 0 and the outlet temperature remains stable, reaching the convergence standard, and end the simulation calculation.

8. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The analysis of the condensation heat transfer process by the temperature cloud diagram and the identification of the flow field distribution law by the flow vector diagram include: Make a longitudinal cross-section perpendicular to the liquid inlet flow direction, observe the temperature distribution cloud map in the upper area, and clarify the heat transfer and temperature gradient; Set up a flow vector diagram on the axial symmetry plane of the final model to visually display the flow of gas and liquid phases and observe eddies, backflows, or uneven flow in the flow pattern.

9. The CFD-based liquefied natural gas recondenser structure optimization method according to claim 1, characterized in that: The calculation of the gas-liquid distribution uniformity and adjustment of the baffle structure include: Make a cross section near the outlet of the gas-liquid distribution plate, establish the outlet velocity cloud map, and use the formula Calculate the uniformity of gas-liquid distribution; where v u is the flow velocity of each outlet channel of the gas-liquid distribution plate, is the average flow velocity at the outlet of the distribution plate, U is the distribution uniformity of gas and liquid; According to the calculated gas-liquid distribution uniformity, the structure of the gas phase baffle and the liquid distribution pipe is adjusted; wherein, the adjustment method is to increase the baffle area or increase the distance between the baffle and the inlet and adjust the spacing between the liquid distribution pipe channels.

10. The CFD-based liquefied natural gas recondenser structure optimization device is characterized by: include: The geometric modeling module is used to build the initial model and complete the geometric pre-processing according to the assembly drawing of the liquefied natural gas recondenser; The fluid channel inside the initial model is extracted using pre-processing software, and the solid wall portion is deleted, the fluid domain is divided along the symmetry plane, half of the flow channel is selected as the calculation domain, and the calculation domain is divided into an upper region, a packing layer region, and a lower region; A meshing module is used to create locally encrypted geometric bodies for key areas, generate an intermediate model, import the intermediate model into a meshing tool, generate a polyhedral mesh, perform mesh independence verification, determine the polyhedral mesh size, and generate a final model; wherein the key areas are baffles, gas-liquid distribution plates, and liquid distribution pipes; The model setup and calculation module is used to import the polyhedral mesh into the solver and perform model setup. This includes configuring the multiphase flow model, turbulence model, and porous media model, as well as inputting physical property parameters. The module also sets boundary and wall conditions and configures solver parameters. The module also sets the initial flow field using a hybrid initialization method, establishes flow and temperature monitoring windows to monitor computational convergence, adjusts the transient time step, and runs the simulation until convergence is achieved. The analysis and optimization module is used to analyze the condensation heat transfer process through temperature cloud maps and identify the flow field distribution pattern through flow vector diagrams; calculate the uniformity of gas-liquid distribution and adjust the baffle structure; analyze the curve of the physical quantity field variation along the height of the packing layer area, adjust the tower diameter and the height of the packing layer area, and iteratively improve the performance of the liquefied natural gas recondenser.

Images