Method for forecasting dynamic characteristic numerical values of coarse particle solid-liquid two-phase flow in vertical lifting pipeline

Abstract

The invention discloses a method for forecasting dynamic characteristic values of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, and belongs to the technical field of flow dynamic characteristic value forecasting. In order to solve the problem that the influence of particle motion on surrounding fluid is not considered in the theoretical calculation and numerical simulation of the solid-liquid two-phase flow in the pipe at present, the method comprises the following steps: firstly, carrying out modeling and grid division on a fluid domain; establishing a particle model based on particle material simulation software, and performing discrete control on particles; then based on computational fluid dynamics software, a coupling interface is established through a coupling interface control equation, the computational fluid dynamics software calculates and monitors the state of fluid, the state serves as an external environment of particles and is conveyed to particle material simulation software, and interference caused by movement of the particles is also transmitted to the computational fluid dynamics software through the coupling interface; and based on the initialized coupling interface, the pipeline model and the particle model, realizing coarse particle solid-liquid two-phase flow dynamic characteristic numerical prediction.

Description

Technical Field

[0001] The invention belongs to the technical field of numerical prediction of fluid dynamics characteristics, and in particular relates to a method for numerical prediction of fluid dynamics characteristics of coarse particle solid-liquid two-phase flow. Background Art

[0002] With the rapid development of the global economy, deep-sea mineral resource mining has become the focus of attention around the world. The deep sea contains rich mineral resources, such as polymetallic manganese nodules, cobalt-rich crusts, etc. In addition, the reserves of these ore elements in the deep sea are much higher than on land. Under the premise of not damaging the marine environment, the safe and efficient development of deep-sea ore resources and the completion of the replacement of terrestrial mineral resources are important topics for future research.

[0003] At present, deep-sea mining schemes are mainly divided into four types: trailer 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 internationally as the mining system with the most use value and development prospects. The pipeline lifting mining system uses air or seawater as a medium to lift seabed ore to the surface. Therefore, the fluid flow in the lifting pipeline has obvious solid-liquid two-phase flow characteristics. For this solid-liquid two-phase flow formed by the mixture of ore particles and seawater, in-depth revelation of the flow field characteristics in the pipeline and the particle flow characteristics are of great significance to improving the ore transportation efficiency and ensuring the safe and stable transportation of ore.

[0004] At present, most of the research on solid-liquid two-phase flow in pipes is limited to horizontal pipe research, and the solid-liquid two-phase flow in pipes is regarded as a pseudo-homogeneous flow composed of fine particles, while there are few studies on solid-liquid two-phase flow composed of coarse particles in vertical pipes. In addition, most of the studies on coarse particle solid-liquid two-phase flow in China are based on sensitivity analysis of some influencing parameters, and qualitative research is carried out to reveal pressure loss. The flow characteristics of coarse particle solid-liquid two-phase flow in vertical pipes should be obviously different from those of fine particle pseudo-homogeneous flow in horizontal pipes, and more emphasis should be placed on the quantitative study of particle velocity distribution and concentration characteristic distribution in pipes. The ore particles in the vertical lifting pipe have large particle size and high density (about twice that of water). In the vertical lifting process, their velocity cannot be kept consistent with the water flow velocity, that is, relative to the water flow, the flow velocity of particles or particle groups will produce a more obvious lag phenomenon. At present, the research on the dynamic characteristics of coarse particle solid-liquid two-phase flow in vertical lifting pipes is obviously insufficient, which poses a great threat to the stability and safety of fluid transportation in pipes.

[0005] For the study of the dynamic characteristics of coarse particle solid-liquid two-phase flow in vertical lifting pipelines, the current research methods mainly include model experiments, theoretical calculations, and numerical simulation methods. Compared with the first two research methods, the numerical simulation method has the advantages of low research cost, flexible and adjustable, and is very suitable for large-scale parameter impact analysis in engineering applications. In order to accurately simulate the movement of individual particles, particle concentration, collisions between particles, and collisions between particles and pipe walls, this application adopts a new computational fluid dynamics (CFD)-discrete element model (DEM) coupling simulation method to solve the problem of internal flow field characteristics of coarse particle solid-liquid two-phase flow. This numerical method can well simulate the flow characteristics of coarse particle two-phase fluid in the pipe, thereby providing reliable data basis and technical support for the safe and stable operation of vertical lifting pipelines. Summary of the invention

[0006] The invention aims to solve the problem that the current theoretical calculation and numerical simulation of solid-liquid two-phase flow in a tube do not consider the influence of the movement of particles themselves on the surrounding fluid.

[0007] A method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline comprises the following steps:

[0008] Step 1: Model the vertical lifting pipeline based on the 3D parametric modeling tool, ignore the wall thickness, take the pipeline model as the fluid domain, and divide the mesh into it;

[0009] Step 2: Establish a particle model based on particle material simulation software and perform discrete control on the particles;

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

[0011] In the process of establishing the coupling interface through the coupling interface control equation, the calculation of fluid and particles is separated based on the UDF function in the computational fluid dynamics software; the computational fluid dynamics software calculates and monitors the state of the fluid and transmits it to the particle material simulation software as the external environment of the particles; and the interference caused by the movement of the particles is also transmitted to the computational fluid dynamics software by the coupling interface to complete the real-time exchange of energy and momentum. The coupling interface control equation includes the fluid control equation and the 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 on the particle is determined as:

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

[0014] Among them, F c 、F fp The contact force between particles and the force exerted by the fluid on the particles are obtained from the momentum equation of the particles; F d is the drag force of the fluid on the particle obtained by the drag force model of the fluid on the particle, F l is the lift obtained by the Saffman lift model;

[0015] Step 4: Based on the initialized coupling interface, pipeline model and particle model, the numerical prediction of the dynamic characteristics of coarse particle solid-liquid two-phase flow is realized.

[0016] Furthermore, when modeling in step 1, the surface segmentation and stretching functions are used to separate the central area of ​​the fluid domain from other areas, and the data is updated to the meshing tool for meshing to complete the encryption work.

[0017] Furthermore, the process of establishing a particle model based on particle material simulation software in step 2 includes the following steps:

[0018] Define particles in the particle material simulation software: Discretely control the particles in the particle material simulation software, define the particles, set the size of coarse particles and fine particles, the size of coarse particles is larger than the size of fine particles, set the material of coarse particles and fine particles to be the same, set the physical properties of the material, and set the percentage of coarse particles and fine particles; at the same time, set the collision recovery coefficient, static friction coefficient and rolling friction coefficient between the particles and the tube wall;

[0019] Define the pipeline geometry in the granular material simulation software, treat the pipeline as a rigid pipe, and set the pipeline material and the physical properties of the material;

[0020] Define the pellet plant, physical model, and set the step size and computational grid in the pellet material simulation software.

[0021] Furthermore, the fluid control equation is controlled by using the Reynolds transport averaged NS equation with added disturbance terms.

[0022] Furthermore, the momentum equation of the particle is:

[0023]

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

[0025] Furthermore, 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:

[0026]

[0027] Among them: 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 particle; V r is the relative velocity of the particles.

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

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

[0030]

[0031] Where: 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 vorticity of the fluid; × represents vector cross product;

[0032] When 1≤Re≤40, using Mei's correlation correction, the lift is:

[0033]

[0034] Where: α = 0.5·Re·ò 2 ;

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

[0036]

[0037] Furthermore, during the initialization of the coupling interface, the coupling interface is imported into FLUENT and initialized:

[0038] After the coupling interface is established, it is imported from the UDF function column of Fluent. Then the boundary conditions, initial conditions, and pre-processing of the structure are all completed in Fluent. The specific 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 boundary properties:

[0043] Since EDEM software can only recognize wall-type interfaces when reading geometry files, you need to change the drawn geometry boundary type in advance, and then export the boundary file and save it in the EDEM folder. The specific operations are as follows:

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

[0045] (303) Fluent grid initialization:

[0046] Import the drawn mesh file in Fluent, click check to check the quality of the mesh, and then initialize the mesh. Enter mesh, reorder, and rd in sequence until the calculation result is close to 1. The above steps are conducive to improving the speed of simulation calculation; because EDEM can only recognize wall-type boundaries, modify the boundary conditions in FLUENT. Double-click Boundary Conditions in the function area, change the type of inlet and outlet to wall, and then output it as a mesh file. Copy the file to the EDEM working folder to prepare for the subsequent EDEM to read the geometric body calculation domain. The specific operations are 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 in the Model column to open the self-defined coupling interface and select Eulerain; then select the drag force model and lift model to be used in turn;

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

[0053] (306) Definition of fluid type:

[0054] Change the default air in Fluent to liquid phase water, set the density ρ, kinematic viscosity υ, inlet velocity V, turbulence intensity, and water particle diameter; the specific operations are as follows:

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

[0056] (307) Turbulence model settings:

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

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

[0059] (308)Phase parameter settings:

[0060] In Fluent, the momentum of the fluid phase is set, and the momentum of the particles is set to zero by default, which is given by EDEM. The operation is 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>Hydraulic Diameter;

[0065] Boundary Conditions>outlet>fluid>Specification Method>Intensity andHydraulicDiameter>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 NS control equation;

[0068] (311) Residual convergence accuracy setting:

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

[0070] (312) Initialization settings:

[0071] For initialization method, select standard initialization processing, for calculation area, select all areas, and then click calculate; the operation is as follows:

[0072] Initialization>all-zone>OK;

[0073] (313) Fluent step size setting:

[0074] Double-click to open the automatic save function, and save each calculation result every N steps. When saving, delete the series of paths before the case name to make the saved path a relative path, that is, automatically save it to the Fluent path. The operation is as follows:

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

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

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

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

[0079] Furthermore, in step (313), during the Fluent step size setting, the calculation time step size is selected to be 1×10 -4 s, and the time step is 15000 steps.

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

[0081] 1. This application innovatively proposes a discrete particle model. Based on this particle model, the physical properties and material properties of the particles can be flexibly and conveniently defined, and the movement 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 pipeline of the deep-sea mining project.

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

[0083] Figure 1 This is the flow chart of numerical simulation of the dynamic characteristics of coarse particle solid-liquid two-phase flow in vertical lifting pipeline;

[0084] Figure 2 Schematic diagram of mesh division for the fluid domain inside the tube;

[0085] Figure 3 is the shear pressure diagram of the wall;

[0086] Figure 4 is the particle position distribution map;

[0087] Figure 5 is the volume fraction of fluid at different cross sections;

[0088] Figure 6 is the velocity field diagram in the pipeline;

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

[0090] Figure 8 This is the dynamic pressure diagram inside the pipeline. DETAILED DESCRIPTION

[0091] This application invents a new type of Euler-Lagrangian method suitable for numerical simulation of coarse particle solid-liquid two-phase flow. This numerical method fully considers the particle shape, particle concentration, collisions between particles and between particles and pipe walls, and can achieve accurate simulation of the flow characteristics of coarse particle solid-liquid two-phase flow, thereby providing strong technical support for the safe and stable operation of vertical lifting pipelines. Compared with the existing technology, the technical solution of this application has the following advantages:

[0092] 1. At present, most of the theoretical calculations and numerical simulation studies on solid-liquid two-phase flow in pipes regard the fluid in the pipe as a homogeneous flow or a pseudo-homogeneous flow composed of fine particles, and do not consider the influence of the movement of the particles themselves on the surrounding fluid. Although this treatment method simplifies the amount of numerical simulation calculations, it cannot deeply reveal the movement characteristics of the flow field inside the pipe. To overcome this challenge, this application innovatively proposes a discrete particle model, which was initially used in agricultural machinery and focused on the movement of particles inside or on the surface of geometric bodies. However, after ANSYS and EDEM are coupled, the fluid provided by ANSYS replaces the position of external air in EDEM, which greatly facilitates the study of the movement characteristics of solid-liquid two-phase flow. Based on this particle model, the physical properties and material properties of the particles can be flexibly and conveniently defined, and the movement 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 work of vertical lifting pipelines in deep-sea mining projects.

[0093] 2. In the current model experimental research on solid-liquid two-phase flow in pipes, due to factors such as high experimental costs and immature experimental technical conditions, researchers usually find it difficult to determine the complex coupling between solid particles in the pipe and the fluid medium in the pipe in the solid-liquid two-phase flow experimental research, which leads to an incomplete understanding of the vibration response mechanism of the vertical pipe under the excitation of solid-liquid two-phase flow. In addition, in the CFD-DEM simulation in recent years, it is mostly used to study the pressure loss inside the pipe, and its post-processing is mostly carried out in FLUENT. The use of EDEM is still insufficient, resulting in an unclear understanding of the vibration characteristics of the particles. In order to overcome this limitation, the present application innovatively proposes a CFD-DEM coupling simulation prediction model, which can complete the coupling of momentum and energy between fluid and particles by setting sub-time steps, and then carry out real-time monitoring of the flow characteristics of solid-liquid two-phase flow in the pipe. The fluid and particles are post-processed in FLUENT and EDEM respectively. This numerical method can accurately and reliably simulate the flow characteristics of coarse particle solid-liquid two-phase flow in vertical lifting pipes. The following is an explanation in conjunction with a specific implementation method. Specific implementation method one:

[0095] This embodiment is a numerical prediction method for the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline. Based on ANSYSFLUENT and EDEM software, a numerical study is conducted on the flow characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline. Figure 1 A flow chart of the numerical simulation method of this application is given.

[0096] The method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline described in this embodiment mainly includes the following steps:

[0097] Step 1: Establish the fluid domain mesh model:

[0098] The present invention focuses on the study of the interaction between the fluid medium and coarse particles in the pipe. In the modeling process, the pipe wall thickness is ignored and the fluid domain is directly meshed.

[0099] In a three-dimensional parametric modeling tool such as DM, the vertical lifting pipeline is modeled. Since the wall thickness is not taken into account, the pipeline model here can be directly regarded as the fluid domain and meshed. The DM is Ansys Design Modeler.

[0100] Fluids have an increasing effect on the velocity of particles. Foreign scholars et al. studied the phase distribution turbulence structure in the solid-liquid two-phase upflow in a vertical pipeline by using two different types of spherical particles, and found that at higher fluid flow rates, there was almost no particle distribution in the near-wall area, that is, when the velocity difference between the particles and the fluid gradually decreased, the particles gathered in the central area of ​​the pipeline. When modeling, the surface segmentation and stretching functions were used to separate the central area of ​​the fluid domain from other areas, and the data was updated to AnsysMeshing for meshing to complete the encryption work.

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

[0102] (101) Import of geometry:

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

[0104] Click WORKBENCH with the left mouse button > a green check mark appears on the right side of Geometry > double-click the Meshing function.

[0105] >Indicates the next step of processing.

[0106] (102) Naming options:

[0107] Enter the Meshing interface, define the boundaries, specify the functions of different surfaces of the geometric body and name them as velocity inlet (inlet), pressure outlet (outlet) and wall (wall) in sequence to complete the preprocessing work of FLUENT reading.

[0108] Click the left mouse button and go to Selection Method > Face Selection > Create Named.

[0109] (103) Grid parameter adjustment:

[0110] Before meshing, adjust the mesh parameters, namely physical preference, smoothness, mesh quality, smoothness, etc., to improve mesh quality and calculation accuracy.

[0111] Click Physics Preferences > Select CFD Options > Select Fluent as the calculation preference;

[0112] Select Mesh Quality > Set to Smooth > High;

[0113] Select Sizing Module > Capture Curvature > On.

[0114] (104)Grid method settings:

[0115] Left click on Method Setup > Select Mesh > Insert > Method > Range > Geometry All Selected > Apply > Define > Multi-Zone > Surface Mesh Control Method > Uniform.

[0116] (105) Grid size adjustment:

[0117] After the structure is segmented, the entire geometry is meshed with a unit size of 12 mm, and the area near the boundary and the center is encrypted with a unit size of 6 mm, and then the mesh is generated. The specific operations are as follows:

[0118] Select Mesh > Insert > Size > Select All Geometries > Apply > Element Size;

[0119] Select Mesh > Insert > Size Adjustment > Selection Method > Select Surface > Geometry Wall > Apply > Element Size Smaller Than Global Element Size;

[0120] Select Mesh > Insert > Sizing > Selection Method > Line Selection > Inlet Center Refine Mesh Boundary Line > Apply > Element Size Smaller Than Global Element Size.

[0121] (106) Grid generation:

[0122] Click Generate Mesh, and the mesh division of the fluid domain in the tube is as follows Figure 2 shown.

[0123] (107) Export file:

[0124] At this point, the meshing has been basically completed, and the encryption of the particle aggregation and the simplification of the approximate layer have been completed. Finally, the mesh file is exported to the FLUENT working path. The specific operations are as follows:

[0125] Select File > Export > Ansys File Output > .mesh File > OK.

[0126] Step 2: Establish particle model based on EDEM software:

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

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

[0129] According to the known working conditions, the diameter of the coarse particles is selected to be close to the maximum size of the grid. When only CFD is used for coarse particle simulation, the diameter of the particles should be less than 10% of the grid size. The purpose is to ensure that the computational grid can capture the dynamic behavior of the particles and avoid the particles "jumping" between grids or failing to correctly express their trajectories. The particle control of the present invention is discretely controlled by EDEM, which overcomes the limitations of the original technology. Therefore, the maximum diameter of the coarse particles can be increased to 0.8 to 0.9 times the maximum grid side length, and the results are still stable and convergent. The fine particles are the same as the minimum grid size, that is, the physical properties of the particles are set as follows: the diameter D is 10 mm and 6 mm, the materials of the coarse particles and the fine particles are the same, the Poisson's ratio υ is 0.3, and the density ρ is 2450 kg / m 3 , Young's modulus is 1×10 7 Pa, the collision recovery 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 percentage of coarse particles is 25%. To simplify the calculation, the pipeline is regarded as a rigid pipe. The pipeline material is high-strength steel, the Poisson's ratio υ is 0.3, and the density ρ is 2500Kg / m 3 , Young's modulus is 1×10 9 Pa, the collision recovery coefficient between the particles and the tube 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] Specify the relationship between particles and geometric bodies:

[0134] Interactions>Particle>CoefficientofRestitution\StaioFriction\RollingFriction;

[0135] Add particles:

[0136] Paticle>NewParticle>PhysicalRadius>SizeDistrinution>fixed>ScaleByRadius\Volume;

[0137] (202) Define the geometry in EDEM:

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

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

[0140] Define the physical properties of the geometry:

[0141] EqupmentMaterial>pipe>Possion'sRatio\SolidsDensity\Young'sModulus;

[0142] Import the fluid domain mesh file:

[0143] Geometries>ImportGeometries>.mesh;

[0144] Table 1. Summary of properties

[0145]

[0146] Table 2. Interaction parameters

[0147]

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

[0149] Click the Geomertrise drop-down option, select ImportGeomertry, that is, in the .mesh file processed by Fluent, and rename each face. Since the types of faces have been adjusted in FLUENT, the design process of the particle factory is simplified here. There is no need to establish a particle generation surface, and the import surface can be directly used as the particle generation surface. According to the assumed particle inlet concentration calculation, there is no limit on the number of particles, 5000 particles are generated per second, and the number of attempts to place particles is set to 20 times to avoid excessive calculations and successful generation of particles. The specific operations are 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 removed smoothly when they reach the outlet surface to avoid blockage in the pipe and affect the calculation accuracy. In addition, when calculating pipeline flow problems, the influence of gravity on the overall flow field is small and can be ignored, so gravity is no longer applied.

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

[0154] Physics>Interaction>Modle;

[0155] Environment>Domain>Gravity.

[0156] (205) Setting the step size in EDEM:

[0157] Enter the Simulation interface, cancel the AutoTimeStep option, set the CurrentStep to 5e-5s, and the time interval should be set so that the results of the coupling between the two can be saved and corresponded smoothly; in addition, the RelyeighPercentage at 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 computational grid in EDEM:

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

[0163] Step 3: Establish coupling interface and initialization based on FLUENT software:

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

[0165] Coupling interface control equation: Based on the UDF function in Fluent, the calculation of fluid and particles is separated. Fluent calculates and monitors the state of the fluid and transmits it to EDEM as the external environment of the particles; and the interference caused by the movement of the particles is also transmitted to Fluent by the coupling interface to complete the real-time exchange of energy and momentum. The control equations involved in the present invention are described in detail below:

[0166] The fluid control equation is as follows:

[0167] The vertical lifting pipeline is simplified to an internal flow problem. The internal fluid is considered to be a Newtonian fluid and meets the constant flow and steady-state incompressible conditions 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 NS equation with added interference is used for control. The equation includes the continuity equation and the momentum conservation equation:

[0168]

[0169] Where ▽ is the Laplace operator, f l is the volume fraction of the fluid; V p is the total volume of particles, V g is the grid volume, n is the number of particles overlapping the grid volume, ρ f is the fluid density, u f is the fluid velocity, p is the fluid pressure, g is the gravitational acceleration, f pf is the force exerted by the particle on the fluid.

[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 results differ greatly from the actual situation. Therefore, the translation and rotational motion of the particles need to be considered. In order to realize the real-time energy and momentum exchange between particles and fluids, the present invention performs the momentum changes of the coarse particles themselves and the changes caused by the external influence on them, including the momentum equation, the drag force model of the fluid on the particles, and the Saffman lift model.

[0171] The momentum equation for the particle is:

[0172]

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

[0174] Model of the drag force of fluid on particles:

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

[0176] According to the working conditions, the particle concentration is less than 50% and the particle distribution is relatively uniform, so the Freestream Equation model can be used to calculate the drag force of the fluid on the particles. This model usually uses Stokes' law, assuming that the particles are spherical and the flow is viscous. The drag force formula is as follows:

[0177]

[0178] Among them: 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 particle; V r is the relative velocity of the particles.

[0179] The Freestream Equation model can be applied to the drag force calculation of most solid-liquid two-phase flows. If special working conditions are encountered, researchers can add and select a suitable drag force model in the coupling interface of EDEM and ANSYS FLUENT. In the actual processing process, they can also develop and import a drag force model suitable for a particle bed or a drag force model suitable for a high-concentration flow during the exploration phase.

[0180] Saffman Lift Model:

[0181] The Saffman lift is mainly caused by the velocity gradient and fluid viscosity and can be expressed as follows:

[0182] Original Saffman lift, that is, when the Reynolds number Re < 1:

[0183]

[0184] Where: C saffman is a constant, usually 1.61; 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 vorticity (rotational speed) of the fluid; × represents the vector cross product.

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

[0186]

[0187] Where: α = 0.5·Re·ò 2 ;

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

[0189]

[0190] Get the comprehensive lift:

[0191] Combining the above models, 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 required, such as establishing an operating platform and modifying model equations, you can enter the C language or C++ language program of the coupling interface to make modifications.

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

[0195] After the coupling interface is established, it is imported from the UDF function column of Fluent. Then the boundary conditions, initial conditions, and pre-processing of the fluid are all completed in Fluent. The following are the specific steps:

[0196] (301) Fluent import file:

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

[0198] (302) Fluent changes boundary properties:

[0199] Since EDEM software can only recognize wall-type interfaces when reading geometry files, it is necessary to change the drawn geometry boundary type in advance, and then export the boundary file and save it in the EDEM folder. This is conducive to reading the geometry in EDEM and avoids repeated establishment of particle factory geometry. The specific operations are as follows:

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

[0201] (303) Fluent grid initialization:

[0202] Import the drawn mesh file in Fluent, click check to check the quality of the mesh, and then initialize the mesh, input mesh, reorder, and rd in sequence until the calculation result is close to 1. The above steps are conducive to improving the speed of simulation calculation. Because EDEM can only recognize wall-type boundaries, modify the boundary conditions in FLUENT. Double-click BoundaryConditions in the function area, change the type of inlet and outlet to wall, and then output it as a mesh file, and copy the file to the EDEM working folder to prepare for the subsequent EDEM to read the geometric body calculation domain. The specific operations are 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, double-click in the model column to open the self-defined coupling interface and select Eulerain. Since the coupling interface uses the Euler method for fluid analysis and the Lagrangian method for particles when compiling, whether you choose Eulerain or Lagrangian, it is still the Euler-Lagrangian method as a whole. The difference is that Eulerian takes the volume fraction into account, while Lagrangian does not. Next, select the drag force model DragModels, lift model LiftModels, and heat transfer model HeatTransferModels to be used. Since heat transfer is not involved, only the first two are selected by default.

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

[0209] Modles>OK.

[0210] (306) Definition of fluid type:

[0211] Change the default air in Fluent to liquid water with a density of ρ of 1000Kg / m 3 , kinematic viscosity υ is 0.001m 2 / s, the flow velocity V at the inlet is 3m / s, the turbulence intensity is 5%, and the water particle diameter is 100mm. In order to avoid backflow, the outlet and inlet are generally set the same.

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

[0213] (307) Turbulence model settings:

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

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

[0216] (308)Phase parameter settings:

[0217] In Fluent, the momentum of the fluid phase is set, and the momentum of the particles is set to zero by default, which is given by EDEM. 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>Hydraulic Diameter;

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

[0223] (310)Method settings:

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

[0225] (311) Residual convergence accuracy setting:

[0226] The general residual convergence accuracy is selected to be 1×10 -3However, specific analysis is still required for specific situations. In FLUENT, the detection of the velocity on each axis of the solid phase is cancelled, and only the specific parameters of the fluid are monitored. The rest can be monitored by EDEM for post-processing. In order to reduce the overall calculation amount, the Print to Console option can be cancelled.

[0227] (312) Initialization settings:

[0228] For initialization method, select standard initialization processing, for calculation area, select all areas, and then click calculate. The operation is as follows:

[0229] Initialization>all-zone>OK;

[0230] (313) Fluent step size setting:

[0231] Double-click to turn on automatic saving, and save each calculation result every 500 steps. When saving, delete the series of paths before the case name to make the saved path a relative path, that is, automatically save to the Fluent path. Here you can choose to save by time or by number of steps.

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

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

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

[0235] This completes the operation steps. The following will deal with specific cases.

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

[0237] Numerical example analysis:

[0238] The present invention simulates the working condition of vertically lifting particles in a deep-sea pipeline, where the pipeline length L is 2500 mm, the pipeline diameter D is 500 mm, the seawater inlet velocity V is 2.5 m / s, and the particle radius R is 5 mm and 3 mm respectively.

[0239] Up Figure 3-Figure 4 According to analysis, in the initial stage of particles, the flow field does positive work on the drag force of the particles, and the velocity of the particles increases, but the velocity of the particles does not increase uniformly, that is, there is a velocity difference between the particles, so collisions between particles and between particles and pipe walls are bound to occur in the initial stage, which also makes the initial shear pressure of the wall larger. Researchers can intuitively observe the distribution of particles under different concentrations by setting different particle concentrations at the inlet at the initial moment, providing data support for subsequent pipeline protection maintenance.

[0240] Figure 5 These are the fluid volume distribution diagrams at pipe lengths L of 1.25m, 1.75m and 2.3m respectively. It can be seen from the above figure that as the particles move in the pipe, the speed difference between the particles and the fluid becomes smaller and smaller, and the longer the movement time, the closer the particles are to the center line.

[0241] In addition, the present invention can also monitor the velocity characteristics, turbulence characteristics and pressure distribution of the flow field inside the pipeline under the influence of coarse particles.

[0242] Figure 6 It reflects the velocity characteristics of the flow field inside the pipe after the particles flow through the pipe. At the beginning, the particles absorb energy and the velocity increases, while the fluid does work on the particles, the velocity V decreases, and the collision between the particles also causes the turbulent characteristics of the internal fluid to change. Researchers can determine the main action area of ​​the fluid and particles by judging the magnitude of the change in fluid velocity. Generally speaking, the more the fluid velocity decreases, the greater the degree of interference of the particles on the fluid flow.

[0243] in addition Figure 7 The magnitude of turbulent energy directly represents the degree of interaction between fluid and particles, reflecting the strength of turbulent eddy and the energy distribution of the flow field. It is precisely because of the action of particles that turbulence occurs in the pipe. On the one hand, the speed difference between particles and fluid is large, and on the other hand, the damping effect of particles will also reduce turbulent energy, especially when the particles are coarse or the volume fraction of particles is large. Researchers can reveal the distribution state of particles based on the gradient change of the turbulent energy field. For example, the area where particles agglomerate often corresponds to the area with lower turbulent energy.

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

[0245] The present invention may also have many other embodiments. Without departing from the spirit and essence of the present invention, those skilled in the art may make various corresponding changes and modifications based on the present invention, but these corresponding changes and modifications should all fall within the scope of protection of the claims attached to the present invention.

Claims

1. A method for numerical prediction of the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline, characterized by: The following steps are involved: Step 1: Model the vertical lifting pipeline based on the 3D parametric modeling tool, ignore the wall thickness, take the pipeline model as the fluid domain, and divide the mesh into it; Step 2: Establish a particle model based on particle material simulation software and perform discrete control on the particles; Step 3: Based on computational fluid dynamics software, a coupling interface is established through a coupling interface control equation, and then the coupling interface is initialized; In the process of establishing the coupling interface through the coupling interface control equation, the calculation of fluid and particles is separated based on the UDF function in the computational fluid dynamics software; the computational fluid dynamics software calculates and monitors the state of the fluid and transmits it to the particle material simulation software as the external environment of the particles; and the interference caused by the movement of the particles is also transmitted to the computational fluid dynamics software by the coupling interface to complete the real-time exchange of energy and momentum. The coupling interface control equation includes the fluid control equation and the particle control equation; 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 on the particle is determined as: F total =F l +F d +F fd +F c Among them, F c 、F fp The contact force between particles and the force exerted by the fluid on the particles are obtained from the momentum equation of the particles; F d is the drag force of the fluid on the particle obtained by the drag force model of the fluid on the particle, F l is the lift obtained by the Saffman lift model; Step 4: Based on the initialized coupling interface, pipeline model and particle model, the numerical prediction of the dynamic characteristics of coarse particle solid-liquid two-phase flow is realized.

2. According to claim 1, a method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline is characterized by: When modeling in step 1, the surface segmentation and stretching functions are used to separate the central area of ​​the fluid domain from other areas, and the data is updated to the meshing tool for meshing to complete the encryption work.

3. According to claim 1, a method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline is characterized by: The process of establishing a particle model based on the particle material simulation software described in step 2 includes the following steps: Define particles in the particle material simulation software: Discretely control the particles in the particle material simulation software, define the particles, set the size of coarse particles and fine particles, the size of coarse particles is larger than the size of fine particles, set the material of coarse particles and fine particles to be the same, set the physical properties of the material, and set the percentage of coarse particles and fine particles; at the same time, set the collision recovery coefficient, static friction coefficient and rolling friction coefficient between the particles and the tube wall; Define the pipeline geometry in the granular material simulation software, treat the pipeline as a rigid pipe, and set the pipeline material and the physical properties of the material; Define the pellet plant, physical model, and set the step size and computational grid in the pellet material simulation software.

4. According to claim 1, a method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline is characterized by: The fluid control equation is controlled by the Reynolds transport averaged NS equation with added disturbance terms.

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

6. According to claim 1, a method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline is characterized by: The drag force model of the fluid on the particles adopts the Freestream Equation model. The drag force calculated by the Freestream Equation model is as follows: Among them: 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 particle; V r is the relative velocity of the particles.

7. According to claim 1, a method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline is characterized by: The Saffman lift model is as follows: When the Reynolds number Re<1, the lift is: Where: 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 vorticity of the fluid; × represents vector cross product; When 1≤Re≤40, using Mei's correlation correction, the lift is: Where: α = 0.5·Re·ò 2 ; When Re>40, the lift is:

8. A method for numerically predicting the dynamic characteristics of coarse particle solid-liquid two-phase flow in a vertical lifting pipeline according to any one of claims 4 to 7, characterized in that: During the initialization of the coupling interface, import the coupling interface in FLUENT and complete the initialization: After the coupling interface is established, it is imported from the UDF function column of Fluent. Then the boundary conditions, initial conditions, and pre-processing of the structure are all completed in Fluent. The specific steps are as follows: (301) Fluent import file: Select file>read>mesh>ok; >Indicates the next step of processing; (302) Fluent changes boundary properties: Since EDEM software can only recognize wall-type interfaces when reading geometry files, you need to change the drawn geometry boundary type in advance, and then export the boundary file and save it in the EDEM folder. The specific operations are as follows: Boundary Conditions>inlet>type>wall; Boundary Conditions>outlet>type>wall.File>Write>mesh; (303) Fluent grid initialization: Import the drawn mesh file in Fluent, click check to check the quality of the mesh, and then initialize the mesh. Enter mesh, reorder, and rd in sequence until the calculation result is close to 1. The above steps are conducive to improving the speed of simulation calculation; because EDEM can only recognize wall-type boundaries, modify the boundary conditions in FLUENT. Double-click Boundary Conditions in the function area, change the type of inlet and outlet to wall, and then output it as a mesh file. Copy the file to the EDEM working folder to prepare for the subsequent EDEM to read the geometric body calculation domain. The specific operations are as follows: Check>mesh>reorder>rd>rd; (304)UDF function import coupling interface: User Defined>Functions>Manage>edem_udf>load; (305) Connection of coupling interface: After importing the UDF function, double-click in the Model column to open the self-defined coupling interface and select Eulerain; then select the drag force model and lift model to be used in turn; Modles>EDEM_UNINSIM>Eulerian>Drag Models>Lift Modls>OK; (306) Definition of fluid type: Change the default air in Fluent to liquid phase water, set the density ρ, kinematic viscosity υ, inlet velocity V, turbulence intensity, and water particle diameter; the specific operations are as follows: Materials>Fluid>Air / Water>Desity(constant)>Visosity(constant)>Change>OK; (307) Turbulence model settings: Select the k-ε model for the turbulence model, and select the dispersed calculation in the calculation model position, that is, FLUENT only calculates the fluid, while the particles are monitored by EDEM. Others are default. The operation is as follows: Viscous>K-epsilon>Near-wall Treatment>Turbulence Mutiphase Modle>Dispaered; (308)Phase parameter settings: In Fluent, the momentum of the fluid phase is set, and the momentum of the particles is set to zero by default, which is given 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)Boundary initial condition setting: 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 the second-order derivative mode, which is consistent with the order of the general NS control equation; (311) Residual convergence accuracy setting: In FLUENT, the detection of the velocity on each axis of the solid phase is cancelled, and only the specific parameters of the fluid are monitored, and the rest can be monitored by EDEM post-processing; (312) Initialization settings: For initialization method, select standard initialization processing, select all areas for calculation area, and then click Calculate; the operation is as follows: Initialization>all-zone>OK; (313) Fluent step size setting: Double-click to open the automatic save function, and save each calculation result every N steps. When saving, delete the series of paths before the case name to make the saved path a relative path, that is, automatically save it to the Fluent path. The operation is as follows: CalculationActivities>Autosave>Save Date File Every>Save Associated CaseFiles>File Name; Select the calculation time step and number of time steps as follows: Run Calculation>Time Step Size>Number of Time Steps>Calculates.

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

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

Images