A numerical prediction method for the kinetic characteristic of coarse particle and liquid two-phase flow in vertical lift pipeline

Abstract

The application relates to a numerical prediction method for the flow dynamics characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, and belongs to the technical field of numerical prediction of flow dynamics characteristics. In order to solve the problem that the influence of particle movement on the surrounding fluid is not considered in the current theoretical calculation and numerical simulation of the solid-liquid two-phase flow in the pipeline, the application firstly models and divides the grid of the fluid domain; a particle model is established based on a particle material simulation software, and the particles are controlled in a discrete manner; then, a coupling interface is established based on a computational fluid dynamics software through a coupling interface control equation; the computational fluid dynamics software calculates and monitors the state of the fluid, which is transported to the particle material simulation software as the external environment of the particles; the interference caused by the movement of the particles is also transmitted to the computational fluid dynamics software through the coupling interface; and the numerical prediction of the flow dynamics characteristics of the coarse particle solid-liquid two-phase flow is realized based on the initialized coupling interface, the pipeline model and the particle model.

Description

TECHNICAL FIELD

[0001] The present application belongs to the technical field of numerical prediction of hydrodynamic characteristics, and particularly relates to a method for numerically predicting hydrodynamic characteristics of coarse particle solid-liquid two-phase flow. BACKGROUND

[0002] With the rapid development of global economy, deep-sea mineral resource exploitation has become the focus of the world. Deep sea contains rich mineral resources, such as polymetallic manganese nodules, cobalt-rich crust, etc. In addition, the reserves of these ore elements in deep sea are much higher than those on land. Under the premise of not damaging the marine environment, safe and efficient development of deep-sea mineral resources to replace land mineral resources is an important research topic in the future.

[0003] At present, deep-sea mining schemes mainly include four types: drag bucket mining system, continuous bucket rope mining system, shuttle mining system and pipeline lifting mining system. Compared with the first three types of mining systems, the pipeline lifting mining system is currently recognized as the most valuable and promising mining system. The pipeline lifting mining system uses air or seawater as the medium to complete the work of lifting the seabed ore to the water surface. Therefore, the fluid flow in the lifting pipeline has obvious solid-liquid two-phase flow characteristics. For the solid-liquid two-phase flow formed by mixing of ore particles and seawater, it is of great significance to reveal the flow field characteristics in the pipeline and the particle flow characteristics to improve the ore conveying efficiency and ensure the safe and stable transportation of the ore.

[0004] At present, the research on solid-liquid two-phase flow in the pipeline is mostly limited to horizontal pipeline research, and the solid-liquid two-phase flow in the pipeline is regarded as a pseudo-homogeneous flow composed of fine particles. There are few studies on solid-liquid two-phase flow in vertical pipeline composed of coarse particles. In China, the research on coarse particle solid-liquid two-phase flow is mostly based on sensitivity analysis of some influencing parameters, and qualitative research is carried out to reveal the pressure loss. The flow characteristics of coarse particle solid-liquid two-phase flow in vertical pipeline are obviously different from the pseudo-homogeneous flow of fine particles in horizontal pipeline, and more attention is paid to the quantitative research on the particle velocity distribution and concentration characteristic distribution in the pipeline. In the vertical lifting pipeline, the ore particles have large particle size and large density (about twice that of water), and their velocity cannot keep consistent with the water flow velocity during vertical upward lifting, that is, the particle or particle group flow velocity lags behind the water flow velocity. At present, the research on hydrodynamic characteristics of coarse particle solid-liquid two-phase flow in vertical lifting pipeline is obviously insufficient, which greatly threatens the stability and safety of fluid transportation in the pipeline.

[0005] For the research on the kinetic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, the current research methods mainly include model experiment, theoretical calculation and numerical simulation method. Compared with the first two research methods, the numerical simulation method has the advantages of low research cost, flexible adjustment and the like, and is very suitable for large-scale parameter influence analysis in engineering application. In order to accurately simulate the motion of a single particle, the particle concentration, the collision between particles and the collision between particles and the pipe wall, a new computational fluid dynamics (CFD)-discrete element model (DEM) coupling simulation method is adopted to solve the internal flow field characteristics of the coarse particle solid-liquid two-phase flow, which can well simulate the flow characteristics of the coarse particle two-phase flow in the pipe, and further provide reliable data basis and technical support for the safe and stable operation of the vertical lifting pipeline. SUMMARY

[0006] The present application is to solve the problem that the current theoretical calculation and numerical simulation of the solid-liquid two-phase flow in the pipe do not consider the influence of the motion of the particles on the surrounding fluid.

[0007] A numerical prediction method for the kinetic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, comprising the following steps:

[0008] Step 1, based on a three-dimensional parameterized modeling tool, model the vertical lifting pipeline, the wall thickness is not considered, the pipeline model is taken as a fluid domain, and the grid is divided;

[0009] Step 2, establish a particle model based on a particle material simulation software, and control the particles discretely;

[0010] Step 3, based on a computational fluid dynamics software, a coupling interface is established by coupling interface control equation, and then the coupling interface is initialized;

[0011] In the process of establishing the coupling interface by the coupling interface control equation, based on the UDF function in the computational fluid dynamics software, the calculation of the fluid and the particle is separated; the state of the fluid calculated by the computational fluid dynamics software is monitored as the external environment of the particle and is transported to the particle material simulation software; and the disturbance caused by the motion of the particle is also transmitted to the computational fluid dynamics software by the coupling interface, so as to complete the real-time exchange of energy and momentum, and the coupling interface control equation includes fluid control equation and particle control equation;

[0012] The particle control equation includes the momentum equation of the particle, the drag force model of the fluid on the particle and the Saffman lift model; based on the momentum equation of the particle, the drag force model of the fluid on the particle and the Saffman lift model, the total force acting on the particle is determined as:

[0013] F total =F l +F d +F fd +F c

[0014] where F c , F fp are the contact force between particles and the force of fluid on particles obtained from the momentum equation of particles; F d is the drag force of fluid on particles obtained from the drag force model of fluid on particles, F l is the lift force obtained from the Saffman lift force model;

[0015] Step four, based on the initialized coupling interface, and the pipe model, the particle model realizes the numerical prediction of the kinetic characteristic of the coarse particle solid-liquid two-phase flow.

[0016] Further, when modeling in step one, the center region of the fluid domain is separated from other regions by using surface segmentation and stretching function, and the data is updated to the grid division tool for grid division, completing the encryption work.

[0017] Further, the process of establishing a particle model based on the particle material simulation software in step two comprises the following steps:

[0018] Defining particles in the particle material simulation software: in the particle material simulation software, the particles are discretely controlled, the particles are defined, the sizes of coarse particles and fine particles are set, the size of the coarse particles is larger than that of the fine particles, the materials of the coarse particles and the fine particles are set to be the same, the physical properties of the materials are set, and the percentages of the coarse particles and the fine particles are set; at the same time, the collision restitution coefficient, the static friction coefficient and the rolling friction coefficient between the particles and the pipe wall are set;

[0019] Defining the pipe geometry in the particle material simulation software, regarding the pipe as a rigid pipe, setting the pipe material and the physical properties of the material;

[0020] Defining the particle factory, the physical model in the particle material simulation software, and setting the step size and the calculation grid.

[0021] Further, the fluid control equation is controlled by the Reynolds transport average N-S equation with added disturbance terms.

[0022] Further, the momentum equation of the particles is:

[0023]

[0024] In the formula, m dem is the mass of the particles, F c represents the contact force between particles, u demF represents the velocity of the particle fp F is the force of the fluid on the particle.

[0025] Further, the drag force model of the fluid on the particle adopts the Freestream Equation model, and the drag force calculated by the Freestream Equation model is as follows:

[0026]

[0027] Wherein: F d is the drag force of the fluid on the particle; μ is the viscosity of the fluid; d p is the diameter of the particle; V r is the relative flow velocity of the particle.

[0028] Further, the Saffman lift force model is as follows:

[0029] When the Reynolds number Re < 1, the lift force is:

[0030]

[0031] In the formula: C saffman is a constant; r is the particle radius; μ is the fluid viscosity coefficient; ρ is the fluid density; v is the relative velocity of the particle; ω is the fluid vorticity; × represents the vector cross product;

[0032] When 1≤Re≤40, the lift force is corrected by Mei's correlation, and the lift force is:

[0033]

[0034] In the formula: α = 0.5·Re·ò 2 ;

[0035] When Re>40, the lift force is:

[0036]

[0037] Further, in the process of initializing the coupling interface, the coupling interface is imported into FLUENT and initialized:

[0038] After the establishment of the coupling interface is completed, it is imported from the UDF function column of Fluent, and then the boundary conditions, initial conditions of the fluid, and the pretreatment of the structure are all completed in Fluent. The specific operation steps are as follows:

[0039] (301) Fluent import file:

[0040] Select file>read>mesh>ok;

[0041] > indicates the next step of processing;

[0042] (302) Fluent changes the boundary properties:

[0043] Since the EDEM software can only identify the wall type interface when reading the geometry file, the boundary type of the drawn geometry needs to be changed in advance, and then the boundary file is exported and stored in the EDEM folder. The specific operation is as follows:

[0044] Boundary Conditions>inlet>type>wall;Boundary Conditions>outlet>type>wall.File>Write>mesh;

[0045] (303) Fluent mesh initialization:

[0046] Import the drawn mesh file in Fluent, click check to check the quality of the mesh, and then initialize the mesh. Input mesh, reorder, rd in turn until the calculation result is approximately 1. The above steps are conducive to improving the speed of simulation calculation; Because EDEM can only recognize the wall type boundary, the boundary conditions are modified in FLUENT. Double-click Boundary Conditions in the function area, and modify the types of inlet and outlet to wall. Then output as a mesh file, and copy the file to the EDEM working folder. Prepare for subsequent EDEM reading of the geometry calculation domain. The specific operation is as follows:

[0047] Check>mesh>reorder>rd>rd;

[0048] (304) UDF function import coupling interface:

[0049] User Defined>Functions>Manage>edem_udf>load;

[0050] (305) Connection of coupling interface:

[0051] After importing the UDF function, double-click the self-defined coupling interface in the model column to open it. Select Eulerain; Next, select the drag force model Drag Models and the lift model Lift Models you want to use;

[0052] Modles>EDEM_UNINSIM>Eulerian>Drag Models>Lift Modls>OK;

[0053] (306) Definition of fluid type:

[0054] Modify the default air in Fluent to liquid phase water, set density p, kinematic viscosity v, flow rate V at the inlet, turbulent intensity, and water particle diameter; the specific operation is as follows:

[0055] Materials>Fluid>Air / Water>Desity(constant)>Visosity(constant)>Change>OK;

[0056] (307) Turbulence model setting:

[0057] Select k-epsilon model for turbulence model, and select dispersed calculation in the calculation model position, that is, FLUENT only calculates the fluid, and the particles are monitored by EDEM, and the others are default, as follows:

[0058] Viscous>K-epsilon>Near-wall Treatment>Turbulence Mutiphase Modle>Dispaered;

[0059] (308) Phase parameter setting:

[0060] Set the momentum original phase of the fluid phase in Fluent, and the momentum original phase of the particles is zero by default, which is given by EDEM, as follows:

[0061] Cell Zone Conditions>Pipe>Fluid>Source Terms>X / Y / Z Momentum;

[0062] Cell Zone Conditions>Pipe>Dem>Source Terms>X / Y / Z Momentum>FixedValues;

[0063] (309) Boundary initial condition setting:

[0064] Boundary Conditions>inlet>fluid>Velocity Magnitude>SpecificationMethod>Intensity and Hydraulic Diameter>Turbulent Intensity>HydraulicDiameter;

[0065] Boundary Conditions>outlet>fluid>Specification Method>Intensity and Hydraulic Diameter>Turbulent Intensity>Hydraulic Diameter;

[0066] (310) Method Settings:

[0067] The momentum term is set to the second-order derivative method, which is consistent with the order of the general N-S control equation;

[0068] (311) Residual convergence precision setting:

[0069] In FLUENT, cancel the detection of the velocity of each axis of the solid phase, only monitor the specific parameters of the fluid, and the rest is monitored by EDEM post-processing;

[0070] (312) Initialization Settings:

[0071] Initialization method, select standard initialization processing, calculate the area selection all area, then click calculation; Operation as follows:

[0072] Initialization>all-zone>OK;

[0073] (313) Fluent step size settings:

[0074] Double-click to open autosave, save the calculation result every time, save once every N steps, and delete the series of paths before the case name when saving, so that the save path is a relative path, that is, automatically saved to the Fluent path; Operation as follows:

[0075] CalculationActivities>Autosave>Save Date File Every>Save AssociatedCase Files>File Name;

[0076] Select the calculation time step and the number of time steps, operation as follows:

[0077] Run Calculation>Time Step Size>Number ofTime Steps>Calculates.

[0078] Further, in the residual convergence precision setting process of step (311), the Print to Console option is selected to be cancelled to reduce the overall calculation amount.

[0079] Further, in the process of setting the Fluent step length, the calculation time step is selected as 1x10 -4 s, and the time step is 15000 steps.

[0080] Compared with the prior art, the technical scheme of the application has the following advantages:

[0081] 1. The application innovatively proposes a discrete particle model. Based on the particle model, the physical properties and material properties of the particles can be defined flexibly and conveniently, and the motion characteristics of the particles in the pipe and the flow characteristics of the fluid in the pipe can be accurately and reliably simulated, thereby providing reliable data support for the reasonable design and safe operation of the deep-sea mining engineering vertical lifting pipe.

[0082] 2. The application innovatively proposes a CFD-DEM coupling simulation prediction model. The model can complete the coupling of momentum and energy between the fluid and the particles by setting a sub-time step, thereby monitoring the flow characteristics of the solid-liquid two-phase flow in the pipe in real time. The numerical method can accurately and reliably simulate the flow characteristics of the coarse particle solid-liquid two-phase flow in the vertical lifting pipe. BRIEF DESCRIPTION OF DRAWINGS

[0083] Figure 1 Flowchart for numerical simulation of the hydrodynamic characteristics of the coarse particle solid-liquid two-phase flow in the vertical lifting pipe;

[0084] Figure 2 Schematic diagram of grid division of the fluid domain in the pipe;

[0085] Figure 3 Shear pressure diagram of the wall surface;

[0086] Figure 4 Position distribution diagram of the particles;

[0087] Figure 5 Fluid volume fraction at different cross sections;

[0088] Figure 6 Velocity field diagram in the pipe;

[0089] Figure 7 Turbulent kinetic energy diagram in the pipe;

[0090] Figure 8 Dynamic pressure diagram inside the pipe. DETAILED DESCRIPTION

[0091] The application discloses a new Euler-Lagrange method suitable for numerical simulation of coarse particle solid-liquid two-phase flow, the numerical method fully considers particle shape, particle concentration, collision between particles and collision between particles and a pipe wall, can realize accurate simulation of flow characteristics of the coarse particle solid-liquid two-phase flow, and further provides strong technical support for safe and stable operation of a vertical lifting pipe.

[0092] 1. At present, in the theoretical calculation and numerical simulation research on the solid-liquid two-phase flow in a pipe, the fluid in the pipe is mostly regarded as homogeneous flow or pseudo-homogeneous flow formed by fine particles, and the influence of particle motion on the surrounding fluid is not considered. Although this processing method simplifies the numerical simulation calculation amount, it cannot reveal the motion characteristics of the flow field in the pipe. To overcome this challenge, the application innovatively proposes a discrete particle model, which is initially mostly used in agricultural machinery and focuses on the motion of particles in or on a geometric body. However, after the coupling of ANSYS and EDEM, the fluid provided by ANSYS replaces the position of the external air in EDEM, greatly facilitating the research on the motion characteristics of the solid-liquid two-phase flow. Based on the particle model, the physical properties and material properties of the particles can be flexibly and conveniently defined, and the motion characteristics of the particles in the pipe and the flow characteristics of the fluid in the pipe can be accurately and reliably simulated, thereby providing reliable data support for the reasonable design and safe operation of the vertical lifting pipe in deep-sea mining engineering.

[0093] 2. In the model experiment research on the solid-liquid two-phase flow in a pipe, due to factors such as high experimental cost and immature experimental technical conditions, researchers usually cannot determine the complex coupling effect between the solid particles in the pipe and the fluid medium in the pipe in the solid-liquid two-phase flow experiment research, thereby leading to insufficient understanding of the vibration response mechanism of the vertical pipe under the excitation of the solid-liquid two-phase flow. In recent years, in the CFD-DEM simulation, the research is mostly on the pressure loss in the pipe, the post-processing is mostly carried out in FLUENT, and the use of EDEM is not sufficient, leading to insufficient understanding of the motion characteristics of the particles. To overcome this limitation, the application innovatively proposes a CFD-DEM coupling simulation prediction model. The model can complete the coupling of momentum and energy between the fluid and the particles by setting a sub-time step, thereby monitoring the flow characteristics of the solid-liquid two-phase flow in the pipe in real time. The fluid and the particles are respectively post-processed in FLUENT and EDEM. The numerical method can accurately and reliably simulate the flow characteristics of the coarse particle solid-liquid two-phase flow in the vertical lifting pipe. The specific embodiments are described below. Specific embodiment one:

[0095] The embodiment is a numerical prediction method for kinetic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, based on two software ANSYS FLUENT and EDEM, numerical research is carried out on the flow characteristics of the coarse particle solid-liquid two-phase flow in the vertical lifting pipeline, Figure 1 The flow chart of the numerical simulation method of the application is given.

[0096] The numerical prediction method for kinetic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline mainly comprises the following steps:

[0097] Step 1: Establish the grid model of the fluid domain:

[0098] The application focuses on the research on the interaction between the fluid medium and the coarse particles in the pipeline, and in the modeling process, the thickness of the pipeline wall is ignored, and the grid division is directly performed on the fluid domain.

[0099] In a three-dimensional parameterized modeling tool, such as DM, the vertical lifting pipeline is modeled, and since the wall thickness is not considered, the pipeline model here can be directly considered as the fluid domain, and the grid division is performed on it, and the DM is Ansys DesignModeler.

[0100] The fluid has a lifting effect on the particle velocity, foreign scholars By using two different kinds of spherical particles, the scholars study the phase distribution turbulent structure in the vertical pipeline solid-liquid two-phase upward flow, and find that there is almost no particle distribution in the near-wall region under high fluid flow rate, that is, when the velocity difference between the particles and the fluid gradually decreases, the particles gather to the center region of the pipeline. When modeling, the surface segmentation and stretching function are used to separate the center region of the fluid domain from other regions, and the data is updated to AnsysMeshing for grid division, and the encryption work is completed.

[0101] The specific steps of grid division are as follows:

[0102] (101) Import of geometric body:

[0103] After completing the geometric structure division in DM, the data needs to be updated to Meshing for grid division.

[0104] Left-click the WORKBENCH>Geometry on the right side with a green check mark, and double-click the Meshing function.

[0105] > indicates the next step.

[0106] (102) Naming selection:

[0107] Enter the Meshing interface, define the boundary, specify the function of different faces of the geometric body and name them in turn as inlet, outlet and wall to complete the pre-processing work for FLUENT reading.

[0108] Left-click the mouse to select the mode> select face> create name.

[0109] (103) Mesh parameter adjustment:

[0110] Before meshing, the parameters of the mesh are adjusted, that is, physical preference, smoothness, mesh quality, smoothness, etc., to improve the mesh quality and calculation accuracy.

[0111] Left-click the mouse to select physical preference> select CFD option> select calculation preference as Fluent;

[0112] Select mesh quality> set to smooth> high;

[0113] Select the size adjustment module> capture curvature> open.

[0114] (104) Mesh method setting:

[0115] Left-click the method setting> select mesh> insert> method> range> select all geometry> apply> define> multi-region> surface mesh control method> uniform.

[0116] (105) Mesh size adjustment:

[0117] After the structure is divided, the entire geometry is meshed with a unit size of 12mm, and for the areas near the boundary and the center area, the encryption operation is performed with a unit size of 6mm, and then the mesh is generated. The specific operation is as follows:

[0118] Select mesh> insert> size adjustment> select all geometry> apply> unit size;

[0119] Select mesh> insert> size adjustment> select mode> select face> geometry wall> apply> unit size smaller than overall unit size;

[0120] Select mesh> insert> size adjustment> select mode> line selection> inlet center refined mesh boundary line> apply> unit size smaller than overall unit size.

[0121] (106) Mesh generation:

[0122] Click to generate mesh, and the mesh division of the fluid domain in the pipe is as shown in Figure 2 .

[0123] (107) Export file:

[0124] So far, the mesh division has been basically completed, and the encryption of the particle aggregation place and the simplification of the approximate layer have been completed. Finally, the mesh file is output to the FLUENT working path, and the specific operation is as follows:

[0125] Select File>Export>Ansys file output>.mesh file>OK.

[0126] Step two, establish a particle model based on EDEM software:

[0127] (201) Define the particles in the particle material simulation software EDEM:

[0128] First, complete the definition of the particles, and the analysis process is as follows:

[0129] According to the known working condition, the diameter of the coarse particles is selected to be similar to the maximum size of the mesh. In the case of only CFD for coarse particle simulation, the diameter of the particle should be less than 10% of the size of the mesh. The purpose is to ensure that the calculation mesh can capture the dynamic behavior of the particle, avoid the particle "jumping" between the meshes or unable to correctly express its trajectory. The particle control of the present application is controlled by EDEM, which overcomes the limitations of the prior art. Therefore, the maximum diameter of the coarse particles can be increased to 0.8-0.9 times the maximum mesh length, and the results are still stable and convergent. The fine particles have the same minimum mesh size, that is, the physical properties of the particles are set as follows: the diameter D is 10mm and 6mm, the materials of the coarse particles and the fine particles are the same, the Poisson's ratio υ is 0.3, the density ρ is 2450Kg / m 3 , the Young's modulus is 1×10 7 Pa, the collision restitution coefficient between particles is 0.85, the static friction coefficient is 0.1, and the rolling friction coefficient is 0.01. The percentage of fine particles is 75%, and the coarse particles are 25%. For simplicity of calculation, the pipeline is regarded as a rigid pipe, the pipeline material is high-strength steel, the Poisson's ratio υ is 0.3, the density ρ is 2500Kg / m 3 , the Young's modulus is 1×10 9 Pa, the collision restitution coefficient between particles and the pipe wall is 0.95, the static friction coefficient is 0.1, and the rolling friction coefficient is 0.01.

[0130] The operation steps are as follows, and the specific parameters are set according to the above analysis:

[0131] Set the physical properties of the particles:

[0132] BulkMaterial>AddBulkMaterial>Possion’sRatio\SolidsDensity\Young’sModulus;

[0133] Define the relationship between particles, geometries:

[0134] Interactions>Particle>Coefficient of Restitution\Staio Friction\Rolling Friction;

[0135] Add particles:

[0136] Paticle>New Particle>Physical Radius>Size Distrinution>fixed>Scale By Radius\Volume;

[0137] (202) Define geometries in EDEM:

[0138] The invention does not consider the vibration of the pipeline, and considers the pipeline as a rigid body, and the material is selected as high-strength steel.

[0139] The operation is as follows, and the specific parameters refer to various parameters of high-strength steel:

[0140] Define the physical properties of the geometries:

[0141] Equpment Material>pipe>Possion's Ratio\Solids Density\Young's Modulus;

[0142] Import the fluid domain mesh file:

[0143] Geometries>Import Geometries>.mesh;

[0144] Table 1. Property summary table

[0145]

[0146] Table 2. Interaction parameter table

[0147]

[0148] (203) Define the particle factory in EDEM:

[0149] Click the Geomertrise drop-down option, select Import Geomertry, that is, the.mesh file processed by Fluent, and complete the naming of each face again. Since the face type adjustment is made in FLUENT, the design process of the particle factory is simplified here, and there is no need to establish a particle generation face. According to the assumed particle import concentration calculation, the number of particles is not limited, 5000 particles are generated per second, and the number of attempts to place particles is set to 20 times to avoid excessive calculation and successful generation of particles. The specific operation is as follows:

[0150] Inlet>Type>Virtual>AddFactory>AddDynamicFactory>NewFactory>Unlimited>Target Number>Velocity.

[0151] (204) Define the physical model in EDEM:

[0152] When defining the physical model, add a custom particle removal model to ensure that the particles can be smoothly removed when reaching the outlet face, avoiding the blockage of particles in the pipe and affecting the calculation accuracy; in addition, when calculating the pipe flow problem, the influence of gravity on the overall flow field is small and can be ignored, so the gravity is not applied.

[0153] Then open the Simulation calculation interface and the coupling interface CouplingSever, wait for the coupling control of Fluent, and the operation is as follows:

[0154] Physics>Interaction>Modle;

[0155] Enviroment>Domain>Gravity.

[0156] (205) Set the step in EDEM:

[0157] Enter the Simulation interface, cancel the AutoTimeStep option, set the CurrentStep to 5e-5s, and the set time interval should be such that the results of the coupling can be successfully saved and corresponded; in addition, the RelyeighPercentage under the set time interval needs to be controlled within 20%.

[0158] The total calculation time is completely controlled by Fluent, and EDEM does not participate in the control.

[0159] SimulatorSettings>FixedTimeStep;

[0160] DateSave>TargetSaveInterval.

[0161] (206) Set up the calculation grid in EDEM:

[0162] Click on EsimateCellSize, select the appropriate grid size under the calculation of EDEM, mostly between 2-5Rmin (EDEM grid size is the multiple of the particle size). Then go back to Fluent and click on the calculation to start the simulation. This case only involves monitoring the velocity field, turbulent energy and pressure field of the fluid inside the pipe, as well as the volume fraction of the fluid inside the pipe. If you want to generate a video, you need to set up the dynamic mesh or solution animation in advance.

[0163] Step three, establish the coupling interface and initialization based on FLUENT software:

[0164] First, establish the coupling interface through the coupling interface control equation;

[0165] Coupling interface control equation: based on the UDF function of Fluent, separate the calculation of fluid and particles. Fluent calculates the state of the monitoring fluid as the external environment of the particles and transmits it to EDEM; the disturbance caused by the movement of the particles is also transmitted to Fluent by the coupling interface, completing the real-time exchange of energy and momentum. The control equation involved in the present application will be described in detail as follows:

[0166] The fluid control equation is as follows:

[0167] The vertical lifting pipe is simplified as an internal flow problem, the internal fluid is considered as a Newtonian fluid, and it satisfies the constant flow, steady-state incompressible condition in time and space. In addition, considering the influence of coarse particles on fluid flow, the volume occupied by coarse particles in the solid-liquid two-phase flow cannot be ignored, so the Reynolds transport average N-S equation with disturbance term is used for control, which includes continuity equation and momentum conservation equation:

[0168]

[0169] In the formula, ▽ is the Laplace operator, f l is the volume fraction of the fluid; V p is the total volume of the particles, V g is the grid volume, n is the number of particles overlapping with the grid volume, ρ f is the fluid density, u f is the fluid velocity, p is the fluid pressure, g is the acceleration of gravity, f pf is the force acting on the fluid from the particles.

[0170] Particle control equation: in the EDEM model, due to the large volume of coarse particles, only the particle center method is used to simulate the trajectory of the particles, which makes the simulation result deviate from the actual situation, so the translation and rotation motion of the particles need to be considered, and the invention realizes the real-time energy and momentum exchange between the particles and the fluid, and the momentum change of the particles themselves and the change caused by the influence of the outside environment, including the momentum equation, the drag force model of the fluid on the particles and the Saffman lift model.

[0171] The momentum equation of the particles is:

[0172]

[0173] In the formula, m dem is the mass of the particles, F c represents the contact force between the particles, u dem represents the velocity of the particles, F fp is the force acting on the particles from the fluid.

[0174] Drag force model of the fluid on the particles:

[0175] Since the velocity of the fluid is greater than the velocity of the particles in this working condition, the total force acting on the particles from the fluid is dynamic.

[0176] According to the working condition, the particle concentration is less than 50%, and the particles are uniformly distributed, so the FreestreamEquation (free stream equation) model can be used to calculate the drag force of the fluid on the particles, which usually uses Stokes law, assumes that the particles are spherical and the flow is viscous, and the drag force formula is as follows:

[0177]

[0178] Where: F d is the drag force of the fluid on the particles, μ is the viscosity of the fluid, d p is the diameter of the particles, and V r is the relative flow velocity of the particles.

[0179] The FreestreamEquation (free stream equation) model can be used for drag force calculation of most solid-liquid two-phase flow, if special working conditions are encountered, researchers can develop and select suitable drag force model in the coupling interface of EDEM and ANSYSFLUENT, and in the actual processing process, the drag force model suitable for the particle bed or the drag force model suitable for high concentration flow can also be developed and imported in the exploration stage.

[0180] Saffman lift model (Saffman Lift Model):

[0181] Saffman lift is mainly caused by velocity gradient and fluid viscosity, which can be expressed as the following formula:

[0182] Original Saffman lift, i.e. when the Reynolds number Re < 1:

[0183]

[0184] In the formula: C saffman is a constant, usually 1.61; r is the radius of the particle; μ is the fluid viscosity coefficient; ρ is the fluid density; v is the relative velocity of the particle; ω is the vorticity (rotational speed) of the fluid; × represents the vector cross product.

[0185] When 1 ≤ Re ≤ 40, Mei's correlation correction is used, and the lift can be expressed as:

[0186]

[0187] In the formula: α = 0.5·Re·ò 2 ;

[0188] When Re > 40, the lift can be expressed as:

[0189]

[0190] Get the comprehensive lift:

[0191] Based on the above model, the total force on the particle is combined by vector addition to obtain the total force:

[0192] F total = F l + F d + F fd + F c (9)

[0193] If secondary development of the coupling interface is needed, such as establishing an operation platform and modifying the model equation, the C language or C++ language program of the coupling interface can be entered for modification.

[0194] Then import the coupling interface in FLUENT and complete the initialization:

[0195] After the establishment of the coupling interface, import it from the UDF function column of Fluent, and then complete the boundary conditions, initial conditions, and structure body preprocessing of the fluid in Fluent. The following are the specific operation steps:

[0196] (301) Fluent import file:

[0197] Select file>read>mesh>ok;

[0198] (302) Fluent change boundary properties:

[0199] Since EDEM software can only identify the wall type interface when reading the geometry file, the boundary type of the drawn geometry needs to be changed in advance, and then the boundary file is exported and stored in the EDEM folder, which is conducive to the reading of the geometry in EDEM, and also avoids the repeated establishment of the particle factory geometry. The specific operation is as follows:

[0200] BoundaryConditions>inlet>type>wall;BoundaryConditions>outlet>type>wall.File>Write>mesh.

[0201] (303) Fluent mesh initialization:

[0202] Import the drawn mesh file in Fluent, click check to check the quality of the mesh, then initialize the mesh, input mesh, reorder, rd in turn, until the calculation result is approximately 1. The above steps are conducive to improving the speed of simulation calculation. Because EDEM can only recognize the wall type boundary, the boundary conditions are modified in FLUENT, double-click BoundaryConditions in the function area, change the type of inlet and outlet to wall, then output as a mesh file, and copy the file to the EDEM working folder, prepare for subsequent EDEM reading geometry calculation domain. The specific operation is as follows:

[0203] Check>mesh>reorder>rd>rd.

[0204] (304) UDF function import (coupling interface):

[0205] UserDefined>Functions>Manage>edem_udf>load.

[0206] (305) Connection of coupling interface:

[0207] After importing the UDF function, open the self-defined coupling interface in the model column by double-clicking, and select Eulerain. Since the coupling interface uses the Euler method for fluid analysis and the Lagrangian method for particles during compilation, whether Eulerain or Lagrangian is selected, it is still an Euler-Lagrangian method overall, the difference is that Eulerian considers volume fraction, while Lagrangian does not consider volume fraction. Next, select the drag force model DragModels, lift model LiftModels, and heat transfer model HeatTransferModels to be used in turn, as no heat transfer is involved, only the first two can be selected by default.

[0208] Modles > EDEM_UNINSIM > Eulerian > Drag Models > Lift Modls > Heat Transfer

[0209] Modles > OK.

[0210] (306) Definition of fluid type:

[0211] Modify the default air in Fluent to liquid phase water, density p is 1000 Kg / m 3 , kinematic viscosity υ is 0.001 m 2 / s, inlet flow rate V is 3 m / s, turbulence intensity is 5%, and water particle diameter is 100 mm. To avoid backflow, the outlet and inlet are set the same.

[0212] Materials > Fluid > Air / Water > Desity (constant) > Visosity (constant) > Change > OK.

[0213] (307) Turbulence model setting:

[0214] Select k-ε model for turbulence model, and select dispersed calculation in the calculation model position, that is, FLUENT only calculates the fluid and the particles are monitored by EDEM, the others are default, as follows:

[0215] Viscous > K-epsilon > Near-wall Treatment > Turbulence Mutiphase Modle > Dispaered.

[0216] (308) Phase parameter setting:

[0217] The momentum primitive of fluid phase is set in Fluent, while the momentum primitive of particles is zero by default, given by EDEM, and the operation is as follows:

[0218] Cell Zone Conditions>Pipe>Fluid>Source Terms>X / Y / Z Momentum;

[0219] Cell Zone Conditions>Pipe>Dem>Source Terms>X / Y / Z Momentum>FixedValues.

[0220] (309) Boundary initial condition setting:

[0221] Boundary Conditions>inlet>fluid>Velocity Magnitude>SpecificationMethod>Intensity and Hydraulic Diameter>Turbulent Intensity>HydraulicDiameter;

[0222] Boundary Conditions>outlet>fluid>Specification Method>IntensityandHydraulicDiameter>Turbulent Intensity>Hydraulic Diameter.

[0223] (310) Method setting:

[0224] The first-order calculation method can solve most of the turbulent flow problems, but in order to achieve the purpose of more realistic and reliable calculation results, the momentum term is set to the second-order derivative, which is consistent with the order of the general N-S control equation. The relaxation factor of the Control term is an important parameter for controlling the convergence speed and stability in the iterative solution process. When solving nonlinear equations, it helps to balance the step size of iterative update to avoid numerical instability or divergence. When the calculation diverges, the relaxation factor can be adjusted, but it will indirectly reduce the calculation accuracy.

[0225] (311) Residual convergence precision setting:

[0226] The general residual convergence precision is selected at 1x10 -3But still need to be analyzed in specific cases. In FLUENT, cancel the detection of the speed of solid phase on each axis, only monitor the specific parameters of the fluid, the rest is monitored by EDEM post-processing, in order to reduce the overall amount of calculation, can choose to cancel the Print to Console option.

[0227] (312) initialization settings:

[0228] Initialization method, select standard initialization processing, calculate the region selection all region, then click calculation.

[0229] Initialization>all-zone>OK;

[0230] (313) Fluent step size settings:

[0231] Double-click to open autosave, save the calculation result of each time, save once every 500 steps, delete the series of paths before the case name when saving, so that the save path is a relative path, that is, automatically saved to the Fluent path, here you can choose to save by time or by step.

[0232] CalculationActivities>Autosave>Save Date File Every>Save AssociatedCase Files>File Name;

[0233] Here we choose the calculation time step size as 1×10 -4 s, time step is 15000 steps, operation as follows:

[0234] Run Calculation>Time Step Size>Number ofTime Steps>Calculates.

[0235] The operation steps are finished, the following is combined with specific cases for processing.

[0236] The application is based on the simulation process of FLUENT, monitors the change of the velocity field, pressure field and turbulent energy field of the fluid; based on the post-processing function of EDEM, monitors the velocity, force and position change of the particles, and then obtains the numerical prediction of the kinetic characteristics of the coarse particle solid-liquid two-phase flow in the vertical lifting pipe.

[0237] Numerical example analysis:

[0238] The application simulates the working condition of deep-sea pipeline vertical lifting particles, the pipeline length L is 2500mm, the pipeline diameter D is 500mm, the seawater import speed is V is 2.5m / s, and the particle radius R is 5mm and 3mm respectively.

[0239] On Figures 3-4 Analysis, in the initial stage of particles, the flow field does positive work to the drag force of the particle, and the velocity of the particle increases, but the velocity of the particle is not uniform, that is, there is a velocity difference between the particles, so the collision between the particles and the wall of the particles must occur in the initial stage, which also makes the shear stress of the wall start to be large, researchers can intuitively observe the distribution of particles under different concentrations by setting the initial time particle concentration at the inlet, and provide data support for subsequent pipeline protection maintenance.

[0240] Figure 5 The fluid volume distribution diagram at the pipeline length L is 1.25m, 1.75m and 2.3m respectively, as shown in the figure, with the movement of particles in the pipeline, the velocity difference between particles and fluid is smaller and smaller, and the longer the movement time is, the closer the particles are to the center line position.

[0241] In addition, the application can also monitor the velocity characteristics, turbulent characteristics and pressure distribution of the flow field in the pipeline under the influence of coarse particles.

[0242] Figure 6 Reflects the velocity characteristics of the flow field in the pipeline after the particles flow through the pipeline, at the beginning, due to the absorption of energy by the particles, the velocity increases, and the fluid does work on the particles, the velocity V decreases, and the collision between the particles also changes the turbulent characteristics of the internal fluid, researchers can judge the main action area of the fluid and the particles by judging the size of the fluid velocity change, generally speaking, the more the fluid velocity decreases, the greater the interference degree of the particles to the fluid flow.

[0243] In addition Figure 7 The size of the turbulent energy directly represents the size of the fluid and particle interaction, reflects the strength of the turbulent vorticity and the energy distribution of the flow field. Due to the action of particles, turbulence appears in the pipeline, on the one hand, the velocity difference between particles and fluid is large, on the other hand, the damping effect of particles will also reduce the turbulent energy, especially when the coarse particles or the particle volume fraction is large. Researchers can reveal the distribution state of particles according to the gradient change of the turbulent energy field, such as the particle agglomeration area often corresponds to the area with low turbulent energy.

[0244] Dynamic pressure is a commonly used concept in fluid mechanics, often used to describe the kinetic energy part of fluid motion. It can represent the momentum change of fluid flow and the energy size related to fluid velocity. In CFD-DEM simulation, dynamic pressure can reflect the drag force of fluid on particles. In high-speed flow, larger dynamic pressure may mean larger particle drag force. In addition, researchers can also judge the local flow characteristics of the flow field according to the dynamic pressure field. The increase or decrease of dynamic pressure usually corresponds to the increase or decrease of flow velocity; in turbulent flow, the sharp fluctuation of dynamic pressure may indicate the instability of flow or the fluctuation of turbulence; finally, in the flow separation zone, the dynamic pressure will decrease significantly, indicating the sharp decrease of fluid velocity.

[0245] The present application can also have other various embodiments, and those skilled in the art can make various corresponding changes and modifications according to the present application without departing from the spirit and essence of the present application. However, these corresponding changes and modifications shall all belong to the protection scope of the claims attached to the present application.

Claims

1. A numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe, characterized in that: Includes the following steps: Step 1: Based on a 3D parametric modeling tool, model the vertical lifting pipe, neglecting the wall thickness, treat the pipe model as a fluid domain, and mesh it. Step 2: Establish a particle model based on particulate material simulation software and perform discrete control on the particles; Step 3: Based on computational fluid dynamics software, establish the coupling interface through the coupling interface control equations, and then initialize the coupling interface; In the process of establishing the coupling interface through the coupling interface control equation, the calculation of fluid and particle is separated based on the UDF function function in the computational fluid dynamics software; the computational fluid dynamics software calculates and monitors the state of the fluid, which is then transmitted to the particle material simulation software as the external environment of the particles; and the disturbances caused by the movement of the particles are also transmitted to the computational fluid dynamics software through the coupling interface to complete the real-time exchange of energy and momentum. The coupling interface control equation includes fluid control equation and particle control equation. The governing equations for the particles include the particle momentum equation, the fluid drag force model on the particles, and the Saffman lift model. Based on the particle momentum equation, the fluid drag force model on the particles, and the Saffman lift model, the total force acting on the particles is determined as follows: F total =F l +F d +F fd +F c Among them, F c F fp The contact forces between particles and the forces exerted by the fluid on the particles are obtained from the momentum equation of the particles; F d The drag force F on the particles is obtained from the fluid-particle drag force model. l The lift is obtained from the Saffman lift model; Step 4: Based on the initialized coupling interface, as well as the pipeline model and particle model, realize the numerical prediction of the dynamic characteristics of coarse particle solid-liquid two-phase flow.

2. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: In step one, during modeling, the surface segmentation and stretching functions are used to separate the central region of the fluid domain from other regions, and the data is updated to the mesh generation tool for mesh generation to complete the densification work.

3. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: Step two describes the process of establishing a particle model based on particulate material simulation software, which includes the following steps: In the particulate material simulation software, particles are defined: the particles are discretely controlled and defined, and the sizes of coarse and fine particles are set. The size of coarse particles is larger than that of fine particles. The coarse and fine particles are made of the same material. The physical properties of the material are set, and the percentage of coarse and fine particles is set. At the same time, the collision recovery coefficient, static friction coefficient and rolling friction coefficient between the particles and the pipe wall are set. Define the pipe geometry in the particulate material simulation software, treat the pipe as a rigid pipe, and set the pipe material and its physical properties. Define the particle plant, physical model, step size, and computational grid in the particulate material simulation software.

4. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: The fluid control equations are controlled by Reynolds transport-averaged Navier-Stokes equations with added disturbance terms.

5. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: The momentum equation for the particle is: In the formula, m dem For the mass of the particles, F c u represents the contact force between particles. dem F represents the velocity of the particle. fp This refers to the force exerted by the fluid on the particles.

6. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: The drag force model of the fluid on the particles adopts the Freestream Equation model, and the drag force calculated by the Freestream Equation model is as follows: Wherein: F d d is the drag force of the fluid on the particles; μ is the viscosity of the fluid; d p V is the diameter of the particle; r denoted as the relative velocity of the particles.

7. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 1, characterized in that: The Saffman lift model is as follows: When the Reynolds number Re < 1, the lift is: In the formula: C saffman ρ is a constant; r is the particle radius; μ is the fluid viscosity coefficient; ρ is the fluid density; v is the relative velocity of the particles; ω is the vorticity of the fluid; × represents the vector cross product; When 1 ≤ Re ≤ 40, using the correlation correction of Mei, the lift is: In the formula: α=0.5·Re·ò 2 ; When Re > 40, the lift is:

8. A numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to any one of claims 4 to 7, characterized in that: During the initialization of the coupled interface, import the coupled interface into FLUENT and complete the initialization: After the coupling interface is established, it is imported into Fluent's UDF function section. Then, the fluid boundary conditions, initial conditions, and preprocessing of the structure are all completed within Fluent. The specific steps are as follows: (301) Fluent import file: Select file > read > mesh > ok; > indicates the next step in the process; (302) Fluent changes boundary properties: Since EDEM software can only recognize wall-type interfaces when reading geometry files, it is necessary to change the boundary type of the drawn geometry beforehand, and then export the boundary file and save it to the EDEM folder. The specific steps are as follows: Boundary Conditions>inlet>type>wall; Boundary Conditions>outlet>type>wall.File>Write>mesh; (303) Fluent mesh initialization: Import the drawn mesh file into Fluent, click "check" to check the mesh quality, and then initialize the mesh by sequentially inputting "mesh," "reorder," and "rd" until the calculation result is approximately 1. These steps help improve the simulation speed. Because EDEM can only recognize wall-type boundaries, modify the boundary conditions in Fluent. Double-click "Boundary Conditions" in the ribbon, change the type of both inlet and outlet to "wall," and then output a mesh file. Copy this file to the EDEM working folder to prepare for EDEM to read the geometric calculation domain later. The specific steps are as follows: Check>mesh>reorder>rd>rd; (304) Importing UDF functions into the coupling interface: User Defined>Functions>Manage>edem_udf>load; (305) Connection of the coupling interface: After importing the UDF function, double-click to open the custom coupling interface in the Model column and select Eulerain; then select the drag force model and lift model to be used in sequence. Modles>EDEM_UNINSIM>Eulerian>Drag Models>Lift Modls>OK; (306) Definition of fluid type: Change the default air phase in Fluent to the liquid phase water, and set the density ρ, kinematic viscosity υ, inlet velocity V, turbulence intensity, and water particle diameter; the specific steps are as follows: Materials>Fluid>Air / Water>Desity(constant)>Visosity(constant)>Change>OK; (307) Turbulence model settings: The k-ε turbulence model is selected, and the calculation model is set to distributed calculation, meaning FLUENT only calculates the fluid, while particles are monitored by EDEM. Other settings are left as default. The operation is as follows: Viscous>K-epsilon>Near-wall Treatment>Turbulence Mutiphase Modle>Dispaered; (308) Phase parameter settings: In Fluent, the momentum inertia of the fluid phase is set, while the momentum inertia of the particles is zero by default and is provided by EDEM. The operation is as follows: Cell Zone Conditions>Pipe>Fluid>Source Terms>X / Y / Z Momentum; Cell Zone Conditions>Pipe>Dem>Source Terms>X / Y / Z Momentum>Fixed Values; (309) Setting initial boundary conditions: Boundary Conditions>inlet>fluid>Velocity Magnitude>Specification Method>Intensity and Hydraulic Diameter>Turbulent Intensity>Hydraulic Diameter; Boundary Conditions>outlet>fluid>Specification Method>Intensity and HydraulicDiameter>Turbulent Intensity>Hydraulic Diameter; (310) Method settings: The momentum term is set to a second-order derivative, consistent with the order of the general Navier-Stokes governing equations; (311) Residual convergence accuracy settings: In FLUENT, disable the detection of velocities on each axis of the solid phase and only monitor the specific parameters of the fluid. The rest can be monitored by EDEM post-processing. (312) Initialization settings: For initialization, select standard initialization, choose the entire region for the calculation area, and then click Calculate; the steps are as follows: Initialization > all-zone > OK; (313) Fluent step size setting: Double-click to enable auto-save. Save the results of each calculation every N steps. During saving, remove the path preceding the case name to make the save path a relative path, automatically saving to the Fluent directory. The operation is as follows: CalculationActivities>Autosave>Save Date File Every>Save Associated CaseFiles>File Name; To select the calculation time step and number of time steps, follow these steps: Run Calculation>Time Step Size>Number of Time Steps>Calculates.

9. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 8, characterized in that: In the residual convergence accuracy setting process described in step (311), in order to reduce the overall computational load, the Print to Console option is unchecked.

10. The numerical prediction method for the dynamic characteristics of coarse-particle solid-liquid two-phase flow in a vertical lifting pipe according to claim 8, characterized in that: In step (313), during the Fluent step size setting process, select a calculation time step size of 1×10. -4 s, with a time step of 15000 steps.

Images