A flow field simulation method for distributed ducted fan-wing coupled layout

Abstract

This invention belongs to the field of numerical simulation methods for flow fields, and provides a flow field simulation method for a distributed ducted fan-wing coupled layout, comprising the following steps: Step 1, dividing the computational model into computational domains based on the airframe, moving blades, and stationary blades, and generating computational meshes; Step 2, assembling the airframe mesh, moving blade mesh, and stationary blade mesh obtained in Step 1 together, and solving the quasi-steady flow field of the entire aircraft at different phase angles of the moving blades; Step 3, based on the solution results of Step 2, extracting the flow field information at the interfaces between the moving blade mesh and the airframe mesh, and between the stationary blade mesh and the airframe mesh; Step 4, based on the airframe mesh, averaging the extracted interface flow field information, and assigning the values ​​to the corresponding interfaces of the airframe mesh as boundary conditions to simulate the effect of the fan on the flow field, and solving the overall flow field and aerodynamic forces of the aircraft. The method of this invention ensures that the moving blade and stationary blade meshes do not participate in the flow field calculation, thus significantly improving computational efficiency while maintaining computational accuracy.

Description

Technical Field

[0001] This invention belongs to the field of flow field numerical simulation methods, specifically relating to a flow field simulation method for a distributed ducted fan-wing coupled layout. Background Technology

[0002] Electrification is a major trend in aircraft development. One of the characteristics of electric propulsion is the "scale independence" of the power system, meaning that breaking down a single high-power power system into multiple low-power power systems does not change the power density and efficiency of the power system. Therefore, distributed electric propulsion technology has gradually become a key development direction for many countries. Distributed ducted fan electric propulsion is an important form of distributed electric propulsion and is attracting increasing attention. Distributed ducted fans can improve the equivalent bypass ratio, and deep coupling with the wing can improve the lift-to-drag ratio during climb and cruise phases. Multiple power units provide safety redundancy, and the power difference can be used to adjust flight attitude.

[0003] Currently, numerical simulation methods play a crucial role in explaining flow mechanisms, reducing research costs, and shortening research time, and are widely used, especially in the aerodynamic performance analysis of aircraft. When dealing with engineering problems involving rotating blades like ducted fans, solving the Reynolds-averaged Navier-Stokes (RANS) equations is often used to simulate viscous flow fields to ensure computational accuracy. To improve computational efficiency, the Multiple Reference Frame (MRF) method is often employed to transform unsteady flow fields into quasi-steady flow fields for calculation. However, for distributed ducted fan-wing coupled layouts, the influence of ducted fans on the overall aerodynamic parameters of the aircraft is crucial, requiring the inclusion of the distributed ducted fan mesh in the calculation. In such layouts, the large number of fans and blades in each fan leads to the "curse of the mesh." Furthermore, to simulate viscous effects, a dense boundary layer mesh needs to be generated near the blade walls, resulting in a massive mesh size. Even with MRF-based quasi-steady methods, the computational iteration speed remains slow and the computational cost is high. Furthermore, the ducted fan has intake and exhaust sections of considerable length at both the front and rear. The accuracy of surface pressure prediction in these sections significantly impacts the overall lift and drag torque coefficients of the aircraft, placing high demands on the precision of the solution method. Therefore, to improve analysis and optimization efficiency in aerodynamic optimization design, it is urgent to develop more efficient flow field simulation methods while ensuring computational accuracy. Summary of the Invention

[0004] To address the aforementioned problems in existing technologies, this invention proposes a flow field simulation method for distributed ducted fan-wing coupled layouts. By replacing boundary conditions with flow field information at the interface, the method simulates the effect of the fan on the flow field, thereby avoiding the need to solve for the flow field near the fan blades. This method can effectively improve the efficiency of solving for the flow field and aerodynamic coefficients in three-dimensional distributed ducted fan-wing coupled layouts while ensuring computational accuracy.

[0005] The technical solution provided by this invention is:

[0006] The flow field simulation method for a distributed ducted fan-wing coupled layout includes the following steps:

[0007] Step 1: Divide the computational domain and generate the computational grid for the computational model, specifically:

[0008] The computational domain and mesh are specifically divided into three parts. The first part is a stationary computational domain surrounding the airframe, including the wings, ducts, and far field. This part of the mesh is the airframe mesh, with a cylindrical region cut out at the location of the moving blade and stationary blade within each duct opening. The second part is a cylindrical rotating computational domain surrounding the moving blade. This part of the mesh is the moving blade mesh, and the diameter of the cylindrical rotating computational domain matches the diameter of the cylindrical region cut out in the airframe mesh. The third part is a cylindrical stationary computational domain surrounding the stationary blade. This part of the mesh is the stationary blade mesh, and the diameter of the cylindrical stationary computational domain matches the diameter of the cylindrical region cut out in the airframe mesh. Furthermore, the sum of the lengths of the cylindrical rotating computational domain containing the moving blade and the cylindrical stationary computational domain containing the stationary blade is equal to the length of the cylindrical region cut out in the airframe mesh, ensuring that the moving blade mesh and the stationary blade mesh can be docked and embedded into the corresponding positions of the airframe mesh to assemble them into a whole.

[0009] Step 2: Assemble the computational meshes of the body, moving blades, and stationary blades obtained in Step 1 together, rotate the moving blade mesh to obtain multiple assembled meshes with moving blades at different phase angles, and use the RANS+MRF method to solve the quasi-steady flow field of the whole machine when the moving blades are at different phase angles.

[0010] Step 3: Based on the solution obtained in Step 2, extract the flow field information at each grid point on the interface between the moving blade grid and the body grid, i.e. the interface in front of the moving blade, and the interface between the stationary blade grid and the body grid, i.e. the interface behind the stationary blade.

[0011] Step 4: Based on the body mesh obtained in Step 1 and the interface flow field information obtained in Step 3, perform RANS solution on the flow field of the entire aircraft to obtain the flow field and aerodynamic coefficients of the entire aircraft. The key boundary condition treatment is as follows:

[0012] The flow field information at the interface in front of the moving blade extracted in step 3 at different phase angles is averaged and assigned to the interface between the moving blade and the body mesh, and set as the outlet boundary; the flow field information at the interface behind the stationary blade extracted in step 3 at different phase angles is averaged and assigned to the interface between the moving blade and the stationary blade mesh, and set as the inlet boundary; the effect of the ducted fan on the flow field is simulated through the above outlet boundary and inlet boundary.

[0013] Furthermore, step 2 specifically includes the following sub-steps:

[0014] Step 2.1: Align the moving blade mesh with the stationary blade mesh and embed them into the corresponding positions in the body mesh to assemble them into a single unit. Assuming the moving blade has m blades, the included angle between two blades at the same position is... Divide this included angle into n time points, and rotate the moving blade mesh in each time point. Degree, to obtain n sets of assembly meshes with moving blades at different phase angles;

[0015] Step 2.2: Based on the n sets of assembled meshes with different phase angles of the moving blades obtained in Step 2.1, the RANS+MRF method is used to solve the quasi-steady flow field of the whole machine at different phase angles of the moving blades.

[0016] Furthermore, the flow field information at each grid point on the interface in step 3 includes three-directional velocity, turbulent kinetic energy, and viscous dissipation rate.

[0017] Furthermore, in step 4, the flow field information at the interface where the moving blades are at different phase angles is averaged. Specifically, based on step 2.2, the RANS+MRF method is used to solve the quasi-steady flow field of the entire machine using n sets of assembled grids where the moving blades are at different phase angles, obtaining the flow field at these n time points. Then, the flow field information at the same grid point on the interface of these n flow fields is averaged. Let f be a certain physical quantity in the flow field information, and the expression for the average value is:

[0018]

[0019] Furthermore, in step 4, when solving the flow field for the body mesh, the cylindrical region that is cut out in the middle of the body mesh is set as a solid domain and does not participate in the flow field calculation. That is, the moving blade mesh and the stationary blade mesh are no longer included in the calculation in this step.

[0020] Beneficial effects

[0021] This invention addresses the problems of large mesh size and slow solution speed encountered in solving quasi / unsteady flow fields of distributed ducted fan-wing coupled aircraft. It proposes a flow field simulation method for this configuration. This method extracts flow field information such as velocity, turbulent kinetic energy, and viscous dissipation rate in three directions at the front and rear interfaces of the quasi-steady flow field and applies it to the corresponding positions at the front and rear interfaces of the bladeless mesh. An outlet boundary and an inlet boundary are introduced to simulate the effect of the ducted fan on the flow field. By solving the quasi-steady flow field once, the aerodynamic coefficients of the entire aircraft and the duct under multiple angles of attack and configurations can be accurately solved. Compared to the traditional RANS method, since the moving and stationary blade meshes do not participate in the flow field calculation, it can significantly improve computational efficiency while maintaining computational accuracy. Attached Figure Description

[0022] Figure 1 The following are the solution steps of a flow field simulation method for a distributed ducted fan-wing coupled layout according to the present invention.

[0023] Figure 2 This is a schematic diagram of the distributed ducted fan-wing coupling layout according to an embodiment of the present invention;

[0024] Figure 3 This is a schematic diagram of the computational domain partitioning in an embodiment of the present invention;

[0025] Figure 4 This is a schematic diagram of the wing grid, moving blade grid, and stationary blade grid and their assembly in an embodiment of the present invention;

[0026] Figure 5 for Figure 4 Schematic diagram of section AA in the diagram;

[0027] Figure 6 for Figure 4 Schematic diagram of the BB section in the diagram;

[0028] Figure 7 This is a schematic diagram of the front and rear interfaces of the wing mesh in an embodiment of the present invention;

[0029] Figure 8 A comparison of the wing surface pressure coefficients calculated using the flow field simulation method proposed in this invention and the traditional RANS+MRF method;

[0030] Figure 9 This paper compares the total lift coefficient calculated based on the flow field simulation method proposed in this invention with the traditional RANS+MRF method, and the lift coefficients of the wing component and the duct component.

[0031] Figure 10 This paper compares the total drag coefficient calculated using the flow field simulation method proposed in this invention with the drag coefficients of the wing component and the duct component using the traditional RANS+MRF method.

[0032] Figure 11 This paper compares the total pitching moment coefficient calculated based on the flow field simulation method proposed in this invention with the traditional RANS+MRF method, and the pitching moment coefficients of the wing component and the duct component.

[0033] In the figure: 1-duct; 2-moving blade; 21-rotational computational domain containing the moving blade; 3-stationary blade; 31-stationary computational domain containing the stationary blade; 4-propeller hub; 5-interface between the moving blade mesh and the wing mesh; 6-interface between the stationary blade mesh and the wing mesh; 8-wing; 81-stationary computational domain containing the wing; 82-cylindrical region removed from the stationary computational domain containing the wing; 9-interface between the moving blade mesh and the stationary blade mesh; 10-interface between the stationary blade mesh and the moving blade mesh; 11-interface between the wing mesh and the moving blade mesh; 12-interface between the wing mesh and the stationary blade mesh. Detailed Implementation

[0034] To make the technical problems solved, the technical solutions, and the beneficial effects of this invention clearer and to enable those skilled in the art to better understand the invention, the invention will be further described in detail and in full below with reference to the accompanying drawings and embodiments. It should be understood that the specific embodiments described herein are for illustrative purposes only and are not intended to limit the invention.

[0035] The present invention will now be described in conjunction with specific embodiments, such as... Figure 1 As shown, this embodiment employs a flow field simulation method for a distributed ducted fan-wing coupled layout provided by the present invention to numerically simulate the flow field and aerodynamic parameters of a certain wing section of a distributed ducted fan-wing coupled layout. The calculation model is as follows: Figure 2 As shown, duct 1 is tightly coupled to wing 8. Wing 8 is a rectangular straight wing with a span of 2059 mm and a chord length of 913 mm. Duct 1 has five duct openings located at the trailing edge of the upper surface of wing 8 and is integrated with the wing design. The inner diameter of the duct openings in duct 1 is 150 mm, and the center-to-center distance between the duct openings is 161 mm. The moving blade 2 has 12 blades, and the stationary blade 3 has 6 blades. The calculation state is Ma = 0.1238, the calculation altitude is 1 km, and the calculation angle of attack range is 2°-16°. The specific calculation steps are as follows:

[0036] Step 1: Targeting Figure 2 The computational model shown divides the computational domain and generates a computational grid, specifically as follows:

[0037] like Figure 3 , Figure 4As shown, the computational domain and mesh are specifically divided into three parts. The first part is a stationary computational domain 81 surrounding the wing 8, including the wing 8, duct 1, and far field. This part has a wing mesh, with a cylindrical region 82 removed from the positions containing the moving blade 2 and the stationary blade 3 within each duct opening. In this embodiment, the wing mesh size is 15 million. The second part is a cylindrical rotating computational domain 21 surrounding the moving blade 2. This part has a moving blade mesh, and the diameter of the cylindrical rotating computational domain 21 matches the diameter of the cylindrical region 82 removed from the wing mesh. In this embodiment, the mesh size of the five rotating computational domains is 41 million. The third part is a cylindrical stationary computational domain 31 surrounding the stationary blade 3. This part has a stationary blade mesh, and the diameter of the cylindrical stationary computational domain 31 matches the diameter of the cylindrical region 82 removed from the wing mesh. In this embodiment, the mesh size of the five stationary domains is 21.5 million. Furthermore, the sum of the lengths of the cylindrical rotational computational domain 21 where the moving blade 2 is located and the cylindrical stationary computational domain 31 where the stationary blade 3 is located is equal to the length of the cylindrical region 82 removed from the wing mesh, ensuring that the moving blade mesh and the stationary blade mesh can be docked and embedded into the corresponding positions of the wing mesh to assemble them into a whole. Since the moving blade mesh and the stationary blade mesh have the characteristic of circular array, the strategy adopted when generating the mesh around the moving blade 2 and the mesh around the stationary blade 3 is to first generate the mesh of a single blade, and then circularly array the mesh of the entire blade. In this embodiment, the moving blade 2 has 12 blades; first, a single blade mesh with an angle of 30 degrees is generated, and then this mesh is circularly arrayed to form a complete 12-blade moving blade mesh. The stationary blade has 6 blades; first, a single blade mesh with an angle of 60 degrees is generated, and then this mesh is circularly arrayed to form a complete 6-blade stationary blade mesh.

[0038] Step 2: Assemble the wing mesh, moving blade mesh, and stationary blade mesh obtained in Step 1 around the wing 8, moving blade 2, and stationary blade 3 together. Rotate the moving blade mesh to obtain the assembled mesh for moving blade 2 at different phase angles. Then, use the RANS+MRF method to solve the quasi-steady flow field of the entire wing section for moving blade 2 at different phase angles. This specifically includes the following sub-steps:

[0039] Step 2.1: Assemble the computational mesh, such as Figures 4 to 6 As shown, the moving blade mesh and the stationary blade mesh are docked and embedded into the corresponding positions of the wing mesh to assemble them into a whole. After assembly, the total mesh size is 77.5 million. In this embodiment, the moving blade has 12 blades, and the included angle between two adjacent blades is 30°. This included angle is divided into 6 time points, and the moving blade mesh is rotated by 0°, 5°, 10°, 15°, 20° and 25° respectively to obtain 6 sets of assembled meshes with the moving blade at different phase angles.

[0040] Step 2.2: Based on the six sets of assembled meshes of the moving blades at different phase angles obtained in Step 2.1, the RANS+MRF method is used to solve the quasi-steady flow field of the entire airfoil section of the moving blade 2 at different phase angles. In this embodiment, the calculation state is Ma = 0.1238, the calculation altitude is 1km, and the angle of attack is 6°. The reason for selecting 6° as the reference state is mainly because the overall cruising angle of attack of the aircraft is 6°, and the flow field information at an angle of attack of 6° is of high importance. When solving the flow field at moving blade mesh rotations of 5°, 10°, 15°, 20°, and 25°, the calculation is based on the flow field at moving blade mesh rotation of 0° to improve the flow field calculation efficiency.

[0041] The RANS+MRF method described in step 2.2 is a multi-reference coordinate system method. Specifically, the computational domain is divided into a rotating computational domain 21 containing the moving blade 2, a stationary computational domain 31 containing the stationary blade 3, and a stationary computational domain 81 containing the wing. The NS equations in the rotating coordinate system are solved in the rotating computational domain 21 containing the moving blade 2; the NS equations in the inertial frame are solved in the stationary computational domain 31 containing the stationary blade 3 and the stationary computational domain 81 containing the wing. The rotating and stationary computational domains are joined together through an interface mesh and information is exchanged through this mesh. To facilitate flux calculation and data exchange between the rotating and stationary computational domains, the equations in this embodiment use absolute physical quantities as parameters. In a coordinate system rotating at a constant rotational speed ω, the NS equations in the rotating coordinate system, expressed in terms of absolute velocity, are as follows:

[0042]

[0043] Where Ω represents the control volume. Here, Q represents the boundary of the control volume, F represents the inviscid flux, G represents the viscous flux, and H is the source term of the equation. In this embodiment, the positive X direction is the direction backward along the fan's rotation axis, the positive Y direction is the direction to the right from the pilot's viewpoint, and the positive Z direction is the direction directly above the pilot's viewpoint. Since the rotation axis is parallel to the x-axis, the expression for the source term H is:

[0044]

[0045] Where ρ, u, v, w, and ω represent the gas density, the velocity components in the x, y, and z directions, and the rotational speed of the blade, respectively. When ω = 0, the equations become:

[0046]

[0047] This is the Navier-Stokes equations in an inertial frame of reference.

[0048] In step 2.2 of this embodiment, the solution method for the equation system is the finite volume method, where the inviscid flux is discretized using Roe's FDS (Flux Difference Splitting) scheme, the viscous flux is discretized using the second-order central difference scheme, the turbulence model is the k-ωSST turbulence model, and the time progression is performed using the approximate factorization method; and large-scale parallel computation is performed based on the MPI (Message Passing Interface) parallel strategy.

[0049] Step 3: Based on the solution obtained in Step 2, extract the flow field information at each grid point on the interface 5 between the moving blade grid and the wing grid (i.e., the interface in front of the moving blade) and the interface 6 between the stationary blade grid and the wing grid (i.e., the interface behind the stationary blade); the flow field information includes three-directional velocity, turbulent kinetic energy and viscous dissipation rate.

[0050] In this embodiment, the method for averaging the flow field information at the interface of the moving blades at different phase angles is as follows: Based on step 2.2, the RANS+MRF method is used to solve the quasi-steady flow field of the entire airfoil section using the assembled grids of the six moving blades at different phase angles, obtaining the flow field at these six time points. Then, the flow field information of the six flow fields at the same grid point on the interface is averaged. Let f be a certain physical quantity in the flow field information, and the expression for the average value is:

[0051]

[0052] The subscript "mean" indicates the average.

[0053] Step 4: Based on the wing mesh obtained in Step 1 and the interface flow field information obtained in Step 3, the CFD solution is performed on the flow field of the entire wing section. The governing equation is the NS equation in the inertial frame. The flow field and aerodynamic coefficients of the entire wing are obtained. The calculation state is Ma = 0.1238, the calculation altitude is 1km, and the calculation angle of attack range is 2°-16°.

[0054] Among them, such as Figure 7As shown, the cylindrical region 82 that has been removed from the wing mesh is designated as a solid domain and is not included in the flow field calculation. That is, the moving blade mesh and the stationary blade mesh are no longer included in the calculation in this step. The key boundary condition processing is as follows: the flow field information extracted in step 3 at the interface 5 in front of the moving blade at different phase angles is averaged and assigned to the interface 11 between the moving blade mesh and the wing mesh, and set as the outlet boundary; the flow field information extracted in step 3 at the interface 6 behind the stationary blade at different phase angles is averaged and assigned to the interface 12 between the moving blade mesh and the stationary blade mesh, and set as the inlet boundary; the above outlet boundary and inlet boundary are used to simulate the effect of the ducted fan on the flow field.

[0055] In step 4 of this embodiment, the solution method for the equation system is the finite volume method, wherein the inviscid flux is discretized using Roe's FDS (Flux Difference Splitting) scheme, the viscous flux is discretized using the second-order central difference scheme, the turbulence model is the k-ωSST turbulence model, and the time progression is performed using the approximate factorization method; and large-scale parallel computation is performed based on the MPI (Message Passing Interface) parallel strategy.

[0056] Figure 8 The paper presents a comparison of the airfoil surface pressure coefficient calculated using the flow field simulation method proposed in this invention and the traditional RANS+MRF method. The cross-section is located at the center of the airfoil component. It can be seen that the flow field simulation method for the distributed ducted fan-airfoil coupled layout proposed in this invention has higher calculation accuracy.

[0057] Figure 9 The paper presents a comparison of the total lift coefficient and the lift coefficients of wing components and duct components calculated using the flow field simulation method proposed in this invention and the traditional RANS+MRF method within the angle of attack range of 2°-16°. Figure 10 The paper presents a comparison of the total drag coefficient and drag coefficients of wing components and duct components calculated using the flow field simulation method proposed in this invention and the traditional RANS+MRF method within the angle of attack range of 2°-16°. Figure 11 This paper presents a comparison of the total pitching moment coefficient and the pitching moment coefficients of wing components and duct components calculated using the flow field simulation method proposed in this invention and the traditional RANS+MRF method within an angle of attack range of 2°-16°. Figures 9 to 11 As can be seen, this invention can accurately calculate the aerodynamic coefficients in a large angle-of-attack domain by introducing boundary conditions at the interface based on the flow field information predicted by the RANS+MRF method under a single angle of attack, demonstrating high calculation accuracy.

[0058] Furthermore, the computation time for the flow field is directly proportional to the number of grid cells. In this embodiment, the traditional RANS+MRF method requires 77.5 million grid cells to compute, and approximately 2,600 cores to compute one state. In contrast, the method of this invention requires 15 million grid cells to compute, and approximately 500 cores to compute one state. The method proposed in this invention requires less than 1 / 5 of the core time required by the traditional method to compute one state. It is evident that the method of this invention can significantly improve computational efficiency while ensuring computational accuracy.

[0059] The above description is only a preferred embodiment of the present invention. It should be noted that for those skilled in the art, several improvements and modifications can be made without departing from the principle of the present invention and without creative effort. These improvements and modifications should also be considered within the scope of protection of the present invention.

Claims

1. A flow field simulation method for a distributed ducted fan-wing coupled layout, characterized in that, Includes the following steps: Step 1: Divide the computational domain and generate the computational grid for the computational model, specifically: The computational domain and mesh are divided into three parts. The first part is the static computational domain surrounding the airframe, including the wing, duct, and far field. The mesh generated in this part is the airframe mesh. The second part is the cylindrical rotating computational domain surrounding the moving blade. The mesh generated in this part is the moving blade mesh. The third part is the cylindrical static computational domain surrounding the stationary blade. The mesh generated in this part is the stationary blade mesh. Step 2: Assemble the body mesh, moving blade mesh, and stationary blade mesh obtained in Step 1 together, rotate the moving blade mesh to obtain multiple assembled meshes with moving blades at different phase angles, and use the RANS+MRF method to solve the quasi-steady flow field of the whole machine when the moving blades are at different phase angles. Step 3: Based on the solution obtained in Step 2, extract the flow field information at each grid point on the interface between the moving blade grid and the body grid, i.e. the interface in front of the moving blade, and the interface between the stationary blade grid and the body grid, i.e. the interface behind the stationary blade. Step 4: Based on the body mesh obtained in Step 1 and the interface flow field information obtained in Step 3, perform RANS solution on the flow field of the entire aircraft to obtain the flow field and aerodynamic coefficients of the entire aircraft. The key boundary condition treatment is as follows: The flow field information at the interface in front of the moving blade extracted in step 3 at different phase angles is averaged and assigned to the interface between the moving blade and the body mesh, and set as the outlet boundary; the flow field information at the interface behind the stationary blade extracted in step 3 at different phase angles is averaged and assigned to the interface between the moving blade and the stationary blade mesh, and set as the inlet boundary; the effect of the ducted fan on the flow field is simulated through the above outlet boundary and inlet boundary.

2. The flow field simulation method for a distributed ducted fan-wing coupled layout according to claim 1, characterized in that: In step 1, a cylindrical region is removed from the location of the moving blade and stationary blade in each duct hole within the body mesh. The diameter of the cylindrical rotational computational domain around the moving blade matches the diameter of the cylindrical region removed from the body mesh, and the diameter of the cylindrical stationary computational domain around the stationary blade matches the diameter of the cylindrical region removed from the body mesh. Furthermore, the sum of the lengths of the cylindrical rotational computational domain around the moving blade and the cylindrical stationary computational domain around the stationary blade is equal to the length of the cylindrical region removed from the body mesh.

3. The flow field simulation method for a distributed ducted fan-wing coupled layout according to claim 1, characterized in that, Step 2 includes the following sub-steps: Step 2.1: Connect the moving blade mesh and the stationary blade mesh and embed them into the corresponding positions of the body mesh to assemble them into a whole. Assuming the moving blade has m blades, the included angle between two blades at the same position is... Divide this included angle into n time points, and rotate the moving blade mesh in each time point. Spend, Obtain n sets of assembly meshes with moving blades at different phase angles; Step 2.2: Based on the n sets of assembled meshes with different phase angles of the moving blades obtained in Step 2.1, the RANS+MRF method is used to solve the quasi-steady flow field of the whole machine at different phase angles of the moving blades.

4. The flow field simulation method for a distributed ducted fan-wing coupled layout according to claim 1, characterized in that, In step 3, the flow field information at each grid point on the interface includes three-directional velocity, turbulent kinetic energy, and viscous dissipation rate.

5. The flow field simulation method for a distributed ducted fan-wing coupled layout according to claim 1, characterized in that, The method for averaging the flow field information at the interface with the moving blades at different phase angles in step 4 is as follows: Based on step 2.2, the RANS+MRF method is used to solve the quasi-steady flow field of the entire machine for n sets of assembled grids with moving blades at different phase angles, obtaining the flow field at these n time points. Then, the flow field information at the same grid point on the interface of these n flow fields is averaged. Let f be a certain physical quantity in the flow field information, and the expression for the average value is: The subscript "mean" indicates the average.

6. The flow field simulation method for a distributed ducted fan-wing coupled layout according to claim 1, characterized in that, In step 4, when solving the flow field for the body mesh, the cylindrical region that is cut out in the middle of the body mesh is set as a solid domain and does not participate in the flow field calculation.

Images