A simulation method for flow and heat transfer performance of battery cooler

Abstract

The present invention discloses a method for simulating the flow and heat transfer performance of a battery cooler, comprising the following steps: extracting a fluid domain in a three-dimensional modeling software and importing it into a pre-processing software; meshing the fluid domain using a polyhedron grid, and dividing the fluid domain into three layers of boundary layer grids at the wall; switching to a solver, setting the energy equation, turbulence model, wall function, and multiphase flow model, and importing a pre-established table of working fluid saturation temperature, pressure, and latent heat; assigning physical parameters such as density, viscosity, specific heat, and thermal conductivity that vary with temperature to the fluid domain; setting the inlet flow, outlet pressure, and wall boundary conditions for the model; selecting a solution algorithm, initializing and submitting the calculation, and analyzing the calculation results. The present invention reduces the difficulty and cycle of battery cooler simulation. At the same time, the simulation results can guide the development and design of the battery cooler, avoiding the waste caused by repeated trial production of samples, thereby allowing sufficient time to improve the structure of the battery cooler, and has certain engineering significance.

Description

Technical Field

[0001] The present invention belongs to the technical field of new energy vehicle components, and in particular relates to a method for simulating the flow and heat exchange performance of a battery cooler. Background Art

[0002] The battery cooler is a heat exchange element connecting the battery circuit and the passenger compartment circuit in the thermal management system of new energy vehicles. It is an application of a plate heat exchanger in a thermal management system. It uses the refrigerant in the passenger compartment circuit as the cold fluid and the coolant in the battery circuit as the hot fluid. It utilizes the latent heat of the refrigerant's evaporation phase change to absorb the heat of the coolant, maintaining the battery at the ideal operating temperature. Under normal operating conditions, the refrigerant-side flow channel has a two-phase flow of liquid and gas, while the coolant-side flow channel has a single-phase flow of liquid. A reasonable battery cooler design should minimize the pressure drop within the flow channel while ensuring that the heat exchange rate meets the standard, thereby reducing the pumping power of the water pump and maximizing economic benefits.

[0003] Due to the narrow and fine features of the battery cooler's flow channels, as well as the phase change in the refrigerant-side flow channels, simulations require high computer performance or distort the calculated results. Currently, battery coolers are generally developed through reverse engineering, that is, designing based on experience, testing performance parameters after trial production, and often failing to meet performance requirements in actual development. This often leads to mold repairs or mold scrapping, which wastes manpower and material costs and prolongs the project cycle. Therefore, a reasonable and effective simulation method is of great significance for shortening the battery cooler development cycle and saving development costs.

[0004] Currently, there are few technical literatures related to the simulation of the flow and heat transfer performance of battery coolers or plate heat exchangers. In the simulation method and system of the patented plate heat exchanger with publication number CN110955984A, the outlet temperatures of the hot-side fluid and the cold-side fluid are assumed, and the heat transfer rate of the hot-side fluid is equal to the heat transfer rate of the cold-side fluid is used as the termination condition for iteration to obtain the outlet temperatures of the fluids on both sides. However, this simulation method is only applicable to the working conditions where the working fluids on both sides of the heat exchanger are the same and no phase change occurs. In addition, this simulation method only monitors the inlet and outlet conditions and is suitable for optimizing control strategies. It is impossible to observe the flow field and temperature field inside the heat exchanger in order to design the turbulence generation structure inside the plate heat exchanger. It cannot provide clear and definite engineering guidance in the early stage of battery cooler design and has limitations. Summary of the Invention

[0005] In response to the problems of large simulation calculation amount and low simulation accuracy of battery coolers, the present invention provides a simulation method for the flow and heat exchange performance of battery coolers. This method can obtain more accurate flow and heat exchange performance of battery coolers in a relatively fast time, shorten the development cycle, and save development costs.

[0006] To achieve this goal, the present invention provides a simulation method for the flow and heat transfer performance of a battery cooler. This method analyzes the performance of a single-layer flow channel to infer the overall heat transfer capacity and flow resistance. It also simulates convective heat transfer between solids and fluids using thin-shell heat transfer to avoid the impact of excessive grid counts on computational speed. Furthermore, it approximates the fluid-solid coupled heat transfer process by setting a fixed wall temperature, ignoring temperature changes in the solid domain that are of no concern. This is achieved by the following steps:

[0007] (1) In the 3D modeling software, create a 3D digital model of the battery cooler. Select any two adjacent plates, hide the rest of the plate, and use Boolean operations to extract the fluid domain between the two plates. Stretch and extend the inlet and outlet sections of the fluid domain to prevent backflow during subsequent simulations that could affect the simulation accuracy. After completion, hide the plates and import the fluid domain and extension sections into the pre-processing software separately.

[0008] (2) To ensure the accuracy of CFD simulation, polyhedron meshes are used in the pre-processing software to mesh the fluid domain. The mesh size is controlled within 0.5 mm, and at least three layers of boundary layer meshes are added. Larger meshes are used for relatively regular areas such as the inlet and outlet sections, and smaller meshes are used for irregular areas such as the main heat exchange area.

[0009] (3) After the meshing is completed, import the mesh into the solver, set the reference pressure to the working pressure under the actual working conditions, select the pressure-based solver, steady-state format, check the energy equation, select the Realizablek-epsilon turbulence model and the scalable wall function SWF. If you are analyzing the refrigerant side flow channel, you should also check the mixture multiphase flow model, select the implicit solution volume fraction, set the main phase to the liquid phase, the auxiliary phase to the gas phase, and select the Lee model that describes the evaporation and condensation phase change as the interaction model between the refrigerant gas and liquid phases, and set the saturation parameters corresponding to the refrigerant working fluid. If you are analyzing the coolant side flow channel, you do not need to set the multiphase flow model;

[0010] According to Lee's model:

[0011]

[0012]

[0013] Where: is the mass source term in the fluid continuity equation, S energy is the energy source term in the fluid energy equation, α is the volume fraction, ρ is the density, T is the temperature, coeff is the constant describing the phase change rate, L is the latent heat of phase change, and the subscripts l and sat represent liquid and saturated states, respectively.

[0014] The calculation formula of constant coeff is:

[0015]

[0016] Where: β is the adjustment coefficient, its value is usually 1, d b is the bubble diameter, whose value needs to be determined through specific experimental data, M is the molar mass, R is the ideal gas constant, and the subscript v indicates the gas state.

[0017] The coeff value obtained by the formula is the value under ideal conditions. During simulation, due to reasons such as mesh quality, taking the original value can easily lead to calculation divergence. Appropriately reducing the coeff value can enhance the convergence of the simulation, but it will have a slight impact on the accuracy of the simulation. In actual simulation, the value of this coefficient should be as close to the calculated value as possible while ensuring the convergence of the calculation.

[0018] The calculation formula for the phase change latent heat L is:

[0019]

[0020] Where: They represent the enthalpy values ​​of saturated gas and saturated liquid respectively.

[0021] (4) Define the physical properties of the fluid that change with temperature, and fit the density, specific heat at constant pressure, viscosity, and thermal conductivity of the fluid as functions of temperature. If you are analyzing the refrigerant side flow channel, you need to define the saturated physical properties of the liquid and gaseous phases of the working fluid separately. If you are analyzing the coolant side flow channel, you only need to define the physical properties of the liquid coolant. In addition, the analysis of the refrigerant side flow channel also requires setting the molar mass, reference temperature, and standard state enthalpy of the two phases;

[0022] (5) Define the boundary conditions of the model. Select the mass flow inlet as the inlet of the flow channel and set the mass flow rate according to the actual working conditions. Select the pressure outlet as the outlet and set the gauge pressure to 0 Pa. Select the constant temperature as the boundary condition of the wall of the fluid-solid coupling area and set the temperature to the saturation temperature of the refrigerant under the current working pressure. Set the thin shell heat transfer and create a grid on the surface of the fluid domain to simulate the convective heat transfer between the solid domain and the fluid domain. The number of grid layers is 1 and the thickness is 1 mm.

[0023] (6) Set the pressure-velocity coupling algorithm to Coupled, select Green-Gauss CellBased for the gradient format, select PRESTO for the pressure discretization format, select Compressive for the volume fraction discretization format, select the first-order upwind format for the remaining spatial discretization formats, and check the pseudo-transient option to enhance the convergence of the simulation. After initialization, set the number of simulation iterations and start the simulation to obtain the flow and heat transfer performance calculation results of the battery cooler.

[0024] When extracting the fluid domain in step (1), only a single-layer fluid domain is extracted. The flow and heat transfer performance of the entire battery cooler is inferred through the simulation results of the single-layer fluid domain, avoiding the huge amount of calculation for multi-layer fluid domains and solid domains, thereby reducing the simulation cycle and difficulty. In addition, since the flow channels on the refrigerant side and the coolant side are symmetrical to each other, any two adjacent plates can be taken. After extracting the fluid domain, the inlet and outlet sections are appropriately extended, and the length of the extended section should be 4 to 10 times the hydraulic diameter. This will allow the flow to fully develop during subsequent simulations, avoid backflow, and improve simulation accuracy.

[0025] When setting the saturation parameters corresponding to the refrigerant working medium in step (3), it is necessary to set the saturation pressure, the corresponding saturation temperature and the phase change latent heat, and import the three in the form of a table. The saturation temperature range should at least cover the possible temperature change range of the refrigerant.

[0026] When setting the inlet mass flow rate in step (5), the set flow rate should be the quotient of the actual flow rate of the working fluid and the number of flow channels occupied by the working fluid. When analyzing the refrigerant side flow channel, the inlet gas phase volume fraction should be set to 0. When setting the wall boundary condition, the saturation temperature of the refrigerant is used as the wall temperature boundary condition to reduce the calculation amount of fluid-solid coupled heat transfer. Thin shell heat transfer is set to simulate the convective heat transfer process between solid and fluid.

[0027] When analyzing the simulation results in step (6), the overall heat exchange of the battery cooler is approximately the product of the heat exchange of a single-layer flow channel and the number of flow channels, and the pressure drop is approximately the pressure drop of a single-layer flow channel.

[0028] Compared with the prior art, the present invention can achieve at least the following beneficial effects:

[0029] (1) The difficulty and cycle of battery cooler simulation are reduced. At the same time, the simulation results can guide the development and design of the battery cooler, avoiding the waste caused by repeated trial production of samples, so that there is sufficient time to improve the structure of the battery cooler.

[0030] (2) The present invention proposes a simulation method for the flow and heat transfer performance of a battery cooler, which can observe the internal field of the battery cooler and provide a more accurate outlet operating condition. BRIEF DESCRIPTION OF THE DRAWINGS

[0031] Figure 1 This is a flow chart of a method for simulating the flow and heat exchange performance of a battery cooler provided by an embodiment of the present invention.

[0032] Figure 2 Schematic diagram of the fluid domain and the extended section in an embodiment of the present invention.

[0033] Figure 3 It is a diagram of the fluid domain grid model in an embodiment of the present invention.

[0034] FIG4( a ) is a schematic diagram of pressure variation in a fluid domain along the flow direction in an embodiment of the present invention.

[0035] FIG4( b ) is a schematic diagram of the temperature change of the fluid domain along the flow direction in an embodiment of the present invention.

[0036] Markings in the figure: 1-inlet extension section; 2-outlet extension section; 3-fluid domain. DETAILED DESCRIPTION

[0037] In order to make the purpose and technical solution of the present invention clearer and more specific, the present invention is further described in detail below with reference to the accompanying drawings and embodiments.

[0038] See also Figure 1 The present invention provides a simulation method for the flow and heat transfer performance of a battery cooler, and the implementation steps are as follows:

[0039] Step 1: Create a 3D digital model of the battery cooler in 3D modeling software. Select any two adjacent plates, hide the rest of the model, and use Boolean operations to extract the fluid domain enclosed between the two plates. Stretching and extending the inlet and outlet sections of the fluid domain prevents backflow during subsequent simulations, which can affect simulation accuracy. Once completed, hide the plates and import the fluid domain and extended sections into the pre-processing software.

[0040] Since the flow channels on the refrigerant side and the coolant side are symmetrical to each other, any two adjacent layers of plates can be used.

[0041] When stretching the inlet and outlet sections of the fluid domain, the length of the extension is 4 to 10 times the hydraulic diameter. This allows for full flow development during subsequent simulations, prevents backflow, and improves simulation accuracy. In some embodiments of the present invention, the extension length is set to four times the hydraulic diameter (30.4 mm). Of course, in other embodiments, other values ​​can be set as needed.

[0042] In some embodiments of the present invention, the fluid domain and the extension are shown in FIG. Figure 2 Wherein, reference numeral 1 represents an inlet extension section, reference numeral 2 represents an outlet extension section, and reference numeral 3 represents a fluid domain.

[0043] In some embodiments of the present invention, when extracting the fluid domain, only a single-layer fluid domain is extracted, and the flow and heat transfer performance of the entire battery cooler is inferred through the simulation results of the single-layer fluid domain, avoiding the huge amount of calculation of multi-layer fluid domains and solid domains, thereby reducing the simulation cycle and difficulty.

[0044] Step 2: Use polyhedral meshes to mesh the fluid domain in the pre-processing software and add at least three layers of boundary layer meshes.

[0045] In some embodiments of the present invention, in this step, in order to ensure the accuracy of CFD simulation, when meshing, the mesh size is controlled within 0.5 mm, and three layers of boundary layer mesh are added. For relatively regular places such as the inlet and outlet sections, a larger mesh size is used, and for irregular places such as the main heat exchange area, a smaller mesh size is used. The mesh after division is shown in FIG. Figure 3 .

[0046] Step 3: After meshing is completed, import the mesh into the solver, set the reference pressure to the working pressure under actual working conditions, select the pressure-based solver, steady-state format, check the energy equation, select the Realizable k-epsilon turbulence model and the scalable wall function SWF.

[0047] In some embodiments of the present invention, the analysis is focused on the refrigerant side flow channel. Therefore, the mixture multiphase flow model is selected, the implicit solution for volume fractions is chosen, the primary phase is set to the liquid phase, the secondary phase is set to the gas phase, the Lee model describing the evaporation-condensation phase transition is selected as the interaction model between the refrigerant gas and liquid phases, and the saturation parameters corresponding to the refrigerant working fluid are set. If the analysis is focused on the coolant side flow channel, the multiphase flow model does not need to be set.

[0048] According to Lee's model:

[0049]

[0050]

[0051] Where: is the mass source term in the fluid continuity equation, S energy is the energy source term in the fluid energy equation, α is the volume fraction, ρ is the density, T is the temperature, coeff is the constant describing the phase change rate, L is the latent heat of phase change, and the subscripts l and sat represent liquid and saturated states, respectively.

[0052] The calculation formula for the phase change latent heat L is:

[0053]

[0054] Where: They represent the enthalpy values ​​of saturated gas and saturated liquid respectively.

[0055] The calculation formula of constant coeff is:

[0056]

[0057] Where: β is the adjustment coefficient, its value is usually 1, d b is the bubble diameter, whose value needs to be determined through specific experimental data, M is the molar mass, R is the ideal gas constant, and the subscript v indicates the gas state.

[0058] In some embodiments of the present invention, after taking specific values,

[0059]

[0060] The coeff value obtained by the formula is the value under ideal conditions. During simulation, due to reasons such as mesh quality, taking the original value can easily lead to calculation divergence. Appropriately reducing the coeff value can enhance the convergence of the simulation, but it will have a slight impact on the accuracy of the simulation. In actual simulation, the value of this coefficient should be as close to the calculated value as possible while ensuring the convergence of the calculation.

[0061] Step 4: Define the temperature-dependent physical properties of the fluid, fitting the density, specific heat at constant pressure, viscosity, and thermal conductivity of the liquid and gaseous fluids as functions of temperature. If analyzing the refrigerant flow path, define the saturated physical properties of the liquid and gaseous phases separately. If analyzing the coolant flow path, define only the physical properties of the liquid coolant. Additionally, setting the molar mass, reference temperature, and standard state enthalpy of both phases is required for analyzing the refrigerant flow path.

[0062] In some embodiments of the present invention, the refrigerant used is R134a, and its thermophysical properties at 253-293K are fitted. The fitting function is shown in Table 1 below. The molar mass of the two phases is defined as 102 kg / kmol, the liquid phase reference temperature is 263.15K, and the standard state enthalpy is 1.9×10 7 j / kmol, gas phase reference temperature 263.15K, standard state enthalpy 4×10 7 In another embodiment, when analyzing the coolant side channel, only the physical properties of the liquid coolant need to be defined.

[0063] Table 1 R134a physical property parameter fitting (253~293K)

[0064]

[0065] Step 5: Define the boundary conditions of the model. Select the mass flow inlet for the flow channel inlet and set the mass flow rate according to the actual working conditions. Select the pressure outlet for the outlet and set the gauge pressure to 0 Pa. Select the constant temperature for the wall boundary condition of the fluid-solid coupling area and set the temperature to the saturation temperature of the refrigerant at the current working pressure. Set the thin shell heat transfer to simulate the convective heat transfer process between the solid and the fluid. Create a grid on the surface of the fluid domain to simulate the convective heat transfer between the solid domain and the fluid domain, and set the number of grid layers and thickness.

[0066] In some embodiments of the present invention, the refrigerant flow rate of the battery cooler is 20L / min, and the refrigerant side flow channel has a total of 15 layers, which is converted to a mass flow rate of approximately 0.0169kg / s. The outlet is selected as a pressure outlet, the gauge pressure is set to 0Pa, and the wall boundary condition of the fluid-solid coupling area is selected as a constant temperature. The temperature is set to the saturation temperature of the refrigerant at the current working pressure of 199418Pa, that is, 263K. Thin shell heat transfer is set, and a grid is created on the surface of the fluid domain to simulate convective heat transfer between the solid domain and the fluid domain. The grid layer number is 1 and the thickness is 1mm.

[0067] Step 6: Set the pressure-velocity coupling algorithm to Coupled, select Green-GaussCellBased for the gradient format, select PRESTO for the pressure discretization format, select Compressive for the volume fraction discretization format, select the first-order upwind format for the remaining spatial discretization formats, and check the pseudo-transient option to enhance the convergence of the simulation. After initialization, set the number of simulation iterations and start the simulation to obtain the flow and heat transfer performance calculation results of the battery cooler.

[0068] In some embodiments of the present invention, analysis of the refrigerant-side flow channel revealed a single-layer heat transfer capacity of 0.567 kW, resulting in an overall battery cooler heat transfer capacity of approximately 8.5 kW and a pressure drop of 28 kPa. Pressure and temperature were analyzed at five sampling points along the flow direction within the main heat exchange zone of the fluid domain to observe pressure and temperature changes within the battery cooler and verify the reliability of the simulation. The results are shown in Figure 4.

[0069] The above description of the disclosed embodiments is intended to enable one skilled in the art to implement or use the present invention. Various modifications to these embodiments will be readily apparent to those skilled in the art, and the general principles defined herein may be implemented in other embodiments without departing from the spirit or scope of the present invention. Therefore, the present invention is not limited to the embodiments shown herein but is intended to conform to the widest scope consistent with the principles and novel features disclosed herein.

Claims

1. A simulation method for flow and heat transfer performance of a battery cooler, characterized in that: The following steps are involved: (1) Build a three-dimensional digital model of the battery cooler. Select any two adjacent plates, hide the rest of the plate, extract the fluid domain enclosed between the two plates, and stretch and extend the inlet and outlet sections of the fluid domain. After completion, hide the plates and import the fluid domain and the extension section into the pre-processing software separately. (2) Mesh the fluid domain and add at least three layers of boundary layer meshes; (3) Import the grid into the solver, set the reference pressure to the working pressure under actual working conditions, select the pressure-based solver, steady-state format, check the energy equation, select the Realizable k-epsilon turbulence model and the scalable wall function SWF. If the refrigerant side flow channel is to be analyzed, the mixture multiphase flow model should also be checked, the implicit solution volume fraction should be selected, the main phase should be set to the liquid phase, the auxiliary phase should be set to the gas phase, and the interaction model between the refrigerant gas and liquid phases should be the Lee model that describes the evaporation and condensation phase change. The saturation parameters corresponding to the refrigerant working medium should be set. If the coolant side flow channel is to be analyzed, the multiphase flow model does not need to be set; (4) Define the physical properties of the fluid that change with temperature, and fit the density, constant pressure specific heat, viscosity, and thermal conductivity of the fluid as a function of temperature. If the refrigerant side flow channel is being analyzed, the saturated physical properties of the working fluid in the liquid and gas phases are defined separately. If the coolant side flow channel is being analyzed, only the physical properties of the liquid coolant need to be defined. In addition, the molar mass, reference temperature, and standard state enthalpy of the two phases also need to be set for the analysis of the refrigerant side flow channel. (5) Define the boundary conditions of the model. Select the mass flow inlet as the inlet of the flow channel, set the mass flow rate according to the actual working conditions, select the pressure outlet as the outlet, set the gauge pressure and determine the wall boundary conditions of the fluid-solid coupling area, set the temperature to the saturation temperature of the refrigerant at the current working pressure, set the thin shell heat transfer, create a grid on the surface of the fluid domain to simulate the convective heat transfer between the solid domain and the fluid domain, and set the number of grid layers and thickness; (6) Set the pressure-velocity coupling calculation, gradient format, pressure discretization format, and volume fraction discretization format. For the remaining spatial discretization formats, select the first-order upwind format and check the pseudo-transient option. After initialization, set the number of simulation iterations and start the simulation to obtain the flow and heat transfer performance calculation results of the battery cooler.

2. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: In step (1), the fluid domain is extracted using Boolean operation methods.

3. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: When extracting the fluid domain in step (1), only a single-layer fluid domain is extracted.

4. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: When the inlet and outlet sections of the fluid domain are stretched and extended in step (1), the length of the extended section is 4 to 10 times the hydraulic diameter.

5. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: The Lee model used in step (3) to define the interphase interaction of the refrigerant side flow channel is: Where: is the mass source term in the fluid continuity equation, S energy is the energy source term in the fluid energy equation, α is the volume fraction, ρ is the density, T is the temperature, coeff is the constant describing the phase change rate, L is the latent heat of phase change, and the subscripts l and sat represent liquid and saturated states, respectively.

6. The method for simulating flow and heat transfer performance of a battery cooler according to claim 5, characterized in that: The calculation formula for the constant coeff is Where: β is the adjustment coefficient, its value is usually 1, d b is the bubble diameter, and its value needs to be determined through specific experimental data, M is the molar mass, R is the ideal gas constant, and the subscript v indicates the gas state; The calculation formula for the phase change latent heat L is: Where: They represent the enthalpy values ​​of saturated gas and saturated liquid respectively.

7. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: When setting the saturation parameters corresponding to the refrigerant working medium in step (3), it is necessary to set the saturation pressure, the corresponding saturation temperature and the latent heat of phase change, and import the three in the form of a table. The saturation temperature range should at least cover the possible temperature variation range of the refrigerant.

8. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: When setting the inlet mass flow rate in step (5), the set flow rate should be the quotient of the actual flow rate of the working fluid and the number of flow channels occupied by the working fluid, and when analyzing the refrigerant side flow channel, the inlet gas phase volume fraction should be set to 0.

9. The method for simulating flow and heat transfer performance of a battery cooler according to claim 1, characterized in that: When setting the wall boundary condition in step (5), the saturation temperature of the refrigerant is used as the wall temperature boundary condition.

10. The method for simulating flow and heat transfer performance of a battery cooler according to any one of claims 1 to 9, characterized in that: When analyzing the simulation results in step (6), the heat exchange capacity of the overall battery cooler is the product of the heat exchange capacity of a single-layer flow channel and the number of flow channels, and the pressure drop is the pressure drop of a single-layer flow channel.

Images