《离心泵CFX流场分析教程.ppt》由会员分享，可在线阅读，更多相关《离心泵CFX流场分析教程.ppt（23页珍藏版）》请在三一办公上搜索。
1、Workshop 5Cavitating Centrifugal Pump,Introduction to CFX,Introduction,The Purpose of the tutorial is to model cavitation in a centrifugal pump,which involves the use of a rotation domain and the cavitation model.The problem consists of a five blade centrifugal pump operating at 2160 rpm.The working
2、 fluid is water and flow is assumed to be steady and incompressible.Due to rotational periodicity a single blade passage will be modeled.The initial flow-field will be solved without cavitation.It will be turned on later.,Start Workbench and save the project as centrifugalpump.wbpjDrag CFX into the
3、Project Schematic from the Component Systems toolboxStart CFX-Pre by double clicking SetupWhen CFX-Pre opens,import the mesh by right-clicking on Mesh and selecting Import Mesh ICEM CFDBrowse to pump.cfx5Keep Mesh units in mClick Open,Workbench,Modifying the material properties:Expand Materials in t
4、he Outline treeDouble-click Water On the Material Properties tab change Density to 1000 kg/m3 Change Dynamic Viscosity to 0.001 kg m-1 s-1 under Transport PropertiesClick OK,Creating Working Fluids,Setting up the Fluid Domain,Double-click on Default DomainUnder Fluid and Particle Definitions,delete
5、Fluid 1 and then create a new Fluid named Water LiquidSet Material to WaterCreate another new Fluid named Water VapourNext to the Material drop-down list,click the“”icon,then the Import Library Data icon(on the right of the form),and select Water Vapour at 25 C under the Water Data objectClick OKBac
6、k in the Material panel,select Water Vapour at 25 CClick OK,Setting up the Fluid Domain,Set the Reference Pressure to 0 PaSet Domain Motion to RotatingSet Angular Velocity to 2160 rev min-1Switch on Alternate Rotation ModelMake sure Rotation Axis under Axis Definition is set to Global ZSwitch to the
7、 Fluid Models tab,and set the following:Turn on Homogeneous Model in the Multiphase sectionUnder Heat Transfer set the Option to Isothermal,with a Temperature of 25 CSet Turbulence Option to Shear Stress TransportClick OK,Inlet Boundary Condition,Insert a boundary condition named InletOn the Basic S
8、ettings tab,set Boundary Type to InletSet Location to INLETSet Frame Type to StationarySwitch to the Boundary Details tabSpecify Mass and Momentum with a Normal Speed of 7.0455 m/sSwitch to the Fluid Values tabFor Water Liquid,set the Volume Fraction to a Value of 1For Water Vapour,set the Volume Fr
9、action to a Value of 0Click OK,Outlet Boundary Condition,Inset a boundary condition named OutletOn the Basic Settings tab,set Boundary Type to OpeningSet Location to OUTSet Frame Type to StationarySwitch to the Boundary Details tabSpecify Mass and Momentum using Entrainment,and enter a Relative Pres
10、sure of 600,000 PaEnable the Pressure Option and set it to Opening PressureSet Turbulence Option to Zero GradientSwitch to the Fluid Values tabFor Water Liquid,set the Volume Fraction to a Value of 1For Water Vapour,set the Volume Fraction to a Value of 0Click OK,Periodic Interface,Click to create a
11、n Interface,and name it PeriodicSet the Interface Type to Fluid FluidFor Interface Side 1,set the Region List to DOMAIN INTERFACE 1 SIDE 1 and DOMAIN INTERFACE 2 SIDE 1(use the“”icon and the Ctrl key)For Interface Side 2,set the Region List to DOMAIN INTERFACE 1 SIDE 2 and DOMAIN INTERFACE 2 SIDE 2S
12、et the Interface Models option to Rotational PeriodicityUnder Axis Definition,select Global ZSet Mesh Connection Option to 1:1Click OK,Wall Boundary Conditions,Insert a boundary condition named StationarySet it to be a Wall,using the STATIONARY locationOn the Boundary Details tab,enable a Wall Veloc
13、ity and set it to Counter Rotating WallClick OKIn the Outline Tree,right-click on the Default Domain Default boundary and rename it to MovingThe default behavior for the Moving boundary condition is to move with the rotating domain,so there is nothing that needs to be set,Initialization,Click to ini
14、tialize the solutionOn the Fluid Settings form,set Water Liquid Volume Fraction to Automatic with Value,and set the Volume Fraction to 1Set Water Vapour Volume Fraction to Automatic with Value,and set the Volume Fraction to 0Click OK,Solver Control,Double click Solver Control in the Outline treeSet
15、Timescale Control to Physical timescaleA commonly used timescale in turbomachinery is 1/omega,where omega is the rotation rate in radians per second.You can use an expression to determine a timestep from this.In this case,2/omega will be used to achieve faster convergence.Enter the following express
16、ion in the Physical Timescale box:1/(pi*2160 min-1)Set Residual Target to 1e-5On the Advanced Options tab,turn on Multiphase Control,then turn on Volume Fraction Coupling and set the Option to CoupledClick OK,Output Control,Double Click on Output Control in the Outline treeOn the Monitor tab,turn on
17、 Monitor OptionsUnder Monitor Points and Expressions,create a new object and call it InletPTotalAbsSet Option to ExpressionSpecify the following expression:massFlowAve(Total Pressure in Stn Frame)InletCreate a new object called InletPStatic,and set Option to Expression Specify the following expressi
18、on:areaAve(Pressure)InletClick OK,Solver,Close CFX-Pre and switch to the Workbench Project windowSave the projectNow double click on Solution in the Project Schematic to start the Solver ManagerWhen the Solver Manager opens,click Start RunWhen the solution has completed,close the Solver Manager and
19、return to the Project windowSave the project,Post-processing,View the results in CFD-Post by double clicking Results in the Project SchematicInsert a Contour by clickingFor the Location,click,expand Regions and then select BLADESet Variable to Absolute Pressure from the extended listSet Range to Glo
20、balOn the Render tab switch off Lighting and Show contour LinesClick Apply,Post-processing,Insert another Contour on the HUB location,using the variable Absolute Pressure coloured by Local Range.Turn off Lighting and Show Contour Lines.Insert another Contour on the SHROUD location,using the variable
21、 Absolute Pressure coloured by Local Range.Turn off Lighting and Show Contour Lines.The minimum pressure is above the Saturation Pressure of 2650 Pa for Water here.In the next step,the outlet pressure will be reduced enough to initiate Cavitation.,Adding another Analysis,Close CFD-Post and return to
22、 the Project SchematicClick the arrow next to the A cell and select DuplicateA new CFX project is created as a copy of the firstChange the name of the new Simulation to CavitationUse the arrow next to the A cell to Rename it to No CavitationSave the ProjectDouble-click Setup for the Cavitation simul
23、ation to open CFX-Pre,Physics Modifications,Edit the Default DomainOn the Fluid Pair Models tab set Mass Transfer to Cavitation Set Option to Rayleigh PlessetTurn on Saturation PressureSet a Saturation Pressure of 2650 PaClick OKEdit the Outlet Boundary ConditionOn the Boundary Details tab,set the R
24、elative Pressure to 300,000 PaClick OK,Physics Modifications,Edit Solver ControlSet the Max.Iterations to 150Set the Residual Target to 1e-4Click OKClose CFX-Pre and save the projectIn the Project Schematic,drag cell A3 onto cell B3The non-cavitating solution will be used as the initial guess for th
25、e cavitating solutionDouble-click Solution for the Cavitation systemIn the Solver Manager note that the initial conditions have been provided from the project schematicClick Start Run,Cavitation Solution,There is a significant spike in residuals,in part due to the outlet pressure difference,but also
26、 due to the fact that the absolute pressure is low enough to induce cavitation.When the run completes,close the Solver Manager and return to the Project SchematicSave the projectDouble-click Results for the Cavitation project to openCFD-Post,Post-processing,If it is not enabled,turn on visibility fo
27、r the Wireframe and turn off visibility for any User Locations and PlotsCreate an XY Plane at Z=0.01 mColour it by Absolute Pressure(the variable is available in the Extended List by clicking).Use a Global RangeThe minimum absolute pressure is equivalent to the Saturation Pressure specified earlier,
28、which is a strong hint that some cavitation has occurredChange the Colour Variable to Water Vapour.Volume FractionChange the Colour Map to Blue to White,Post-processing,Turn off visibility for Plane 1Create a Volume using the Isovolume methodSet the Variable to Water Vapour.Volume FractionSet Mode t
29、o Above Value,and enter a value of 0.5To view 360 degrees of the model,double-click Default TransformUncheck Instancing Info from DomainSet#of copies to 5Set#of Passages to 5Click OK,Post-processing,The main area of cavitation exists between the suction side of the blade and the shroud in this geome
30、try.A secondary area of cavitation is just behind the leading edge of the blade on the pressure sideFurther steps to try:Calculate torque on the BLADE using the function calculator(hint,use the extended region list to find the BLADE,and use Global Z axis)Plot velocity Vectors on Plane 1,using the variableWater Liquid.Velocity in Stn.FrameCalculate the mass flow through the pump(hint:use the function calculator to evaluate massFlow at the Outlet region)Using a similar method to step 2,calculate the drop in Total Pressure from Inlet to OutletPlot Streamlines,starting from the Inlet location,
