CFX离心泵算例p学习课程

1、IntroductionThe 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 fluid is water and flow is assumed to be steady and inco

2、mpressible.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. 第1页/共23页第一页，编辑于星期五：十三点 五十四分。1. Start Workbench and save the project as centrifugalpump.wbpj2. Drag CFX into the Project Schematic fro

3、m the Component Systems toolbox3. Start CFX-Pre by double clicking Setup4. When CFX-Pre opens, import the mesh by right-clicking on Mesh and selecting Import Mesh ICEM CFD5. Browse to pump.cfx56. Keep Mesh units in m7. Click OpenWorkbench 第2页/共23页第二页，编辑于星期五：十三点 五十四分。Modifying the material properties

4、:1. Expand Materials in the Outline tree2. Double-click Water 3. On the Material Properties tab change Density to 1000 kg/m3 4. Change Dynamic Viscosity to 0.001 kg m-1 s-1 under Transport Properties5. Click OKCreating Working Fluids第3页/共23页第三页，编辑于星期五：十三点 五十四分。Setting up the Fluid Domain1.Double-cli

5、ck on Default Domain2.Under Fluid and Particle Definitions, delete Fluid 1 and then create a new Fluid named Water Liquid3.Set Material to Water4.Create another new Fluid named Water Vapour5.Next to the Material drop-down list, click the “” icon, then the Import Library Data icon (on the right of th

6、e form), and select Water Vapour at 25 C under the Water Data objectClick OK6.Back in the Material panel, select Water Vapour at 25 CClick OK第4页/共23页第四页，编辑于星期五：十三点 五十四分。Setting up the Fluid Domain7.Set the Reference Pressure to 0 Pa8.Set Domain Motion to Rotating9.Set Angular Velocity to 2160 rev mi

7、n-110. Switch on Alternate Rotation Model11. Make sure Rotation Axis under Axis Definition is set to Global Z11. Switch to the Fluid Models tab, and set the following:12. Turn on Homogeneous Model in the Multiphase section13. Under Heat Transfer set the Option to Isothermal, with a Temperature of 25

8、 C14. Set Turbulence Option to Shear Stress Transport15. Click OK第5页/共23页第五页，编辑于星期五：十三点 五十四分。Inlet Boundary Condition1. Insert a boundary condition named Inlet2. On the Basic Settings tab, set Boundary Type to Inlet3. Set Location to INLET4. Set Frame Type to Stationary5. Switch to the Boundary Deta

9、ils tab6. Specify Mass and Momentum with a Normal Speed of 7.0455 m/s7. Switch to the Fluid Values tab8. For Water Liquid, set the Volume Fraction to a Value of 19. For Water Vapour, set the Volume Fraction to a Value of 010.Click OK第6页/共23页第六页，编辑于星期五：十三点 五十四分。Outlet Boundary Condition1. Inset a bou

10、ndary condition named Outlet2. On the Basic Settings tab, set Boundary Type to Opening3. Set Location to OUT4. Set Frame Type to Stationary5. Switch to the Boundary Details tab6. Specify Mass and Momentum using Entrainment, and enter a Relative Pressure of 600,000 Pa7. Enable the Pressure Option and

11、 set it to Opening Pressure8. Set Turbulence Option to Zero Gradient9. Switch to the Fluid Values tab10.For Water Liquid, set the Volume Fraction to a Value of 111.For Water Vapour, set the Volume Fraction to a Value of 012.Click OK第7页/共23页第七页，编辑于星期五：十三点 五十四分。Periodic Interface1. Click to create an

12、Interface, and name it Periodic2. Set the Interface Type to Fluid Fluid3. For 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)4. For Interface Side 2, set the Region List to DOMAIN INTERFACE 1 SIDE 2 and DOMAIN INTERF

13、ACE 2 SIDE 25. Set the Interface Models option to Rotational Periodicity6. Under Axis Definition, select Global Z7. Set Mesh Connection Option to 1:18. Click OK第8页/共23页第八页，编辑于星期五：十三点 五十四分。Wall Boundary Conditions1.Insert a boundary condition named Stationary2.Set it to be a Wall, using the STATIONAR

14、Y location3.On the Boundary Details tab, enable a Wall Velocity and set it to Counter Rotating Wall4.Click OK5.In 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

15、 there is nothing that needs to be set第9页/共23页第九页，编辑于星期五：十三点 五十四分。Initialization1.Click to initialize the solution2.On the Fluid Settings form, set Water Liquid Volume Fraction to Automatic with Value, and set the Volume Fraction to 13.Set Water Vapour Volume Fraction to Automatic with Value, and se

16、t the Volume Fraction to 04.Click OK第10页/共23页第十页，编辑于星期五：十三点 五十四分。Solver Control1.Double click Solver Control in the Outline tree2.Set 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

17、expression to determine a timestep from this. In this case, 2/omega will be used to achieve faster convergence.3.Enter the following expression in the Physical Timescale box:1/(pi*2160 min-1)4.Set Residual Target to 1e-55.On the Advanced Options tab, turn on Multiphase Control, then turn on Volume F

18、raction Coupling and set the Option to Coupled6.Click OK第11页/共23页第十一页，编辑于星期五：十三点 五十四分。Output Control1.Double Click on Output Control in the Outline tree2.On the Monitor tab, turn on Monitor Options3.Under Monitor Points and Expressions, create a new object and call it InletPTotalAbs4.Set Option to E

19、xpression5.Specify the following expression: massFlowAve(Total Pressure in Stn Frame )Inlet6.Create a new object called InletPStatic, and set Option to Expression 7.Specify the following expression:areaAve(Pressure )Inlet8.Click OK第12页/共23页第十二页，编辑于星期五：十三点 五十四分。Solver1.Close CFX-Pre and switch to the

20、 Workbench Project window2.Save the project3.Now double click on Solution in the Project Schematic to start the Solver Manager4.When the Solver Manager opens, click Start Run5.When the solution has completed, close the Solver Manager and return to the Project window6.Save the project第13页/共23页第十三页，编辑

21、于星期五：十三点 五十四分。Post-processing1.View the results in CFD-Post by double clicking Results in the Project Schematic2.Insert a Contour by clicking3.For the Location, click , expand Regions and then select BLADE4.Set Variable to Absolute Pressure from the extended list5.Set Range to Global6.On the Render

22、tab switch off Lighting and Show contour Lines7.Click Apply第14页/共23页第十四页，编辑于星期五：十三点 五十四分。Post-processing9.Insert another Contour on the HUB location, using the variable Absolute Pressure coloured by Local Range. Turn off Lighting and Show Contour Lines. 10. Insert another Contour on the SHROUD locat

23、ion, using the variable 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.第15页/共23页第十五页，编辑于星期五：十三点 五

24、十四分。Adding another Analysis1.Close CFD-Post and return to the Project Schematic2.Click the arrow next to the A cell and select DuplicateA new CFX project is created as a copy of the first3.Change the name of the new Simulation to Cavitation4.Use the arrow next to the A cell to Rename it to No Cavita

25、tion5.Save the Project6.Double-click Setup for the Cavitation simulation to open CFX-Pre第16页/共23页第十六页，编辑于星期五：十三点 五十四分。Physics Modifications1.Edit the Default Domain2.On the Fluid Pair Models tab set Mass Transfer to Cavitation 3.Set Option to Rayleigh Plesset4.Turn on Saturation Pressure5.Set a Satu

26、ration Pressure of 2650 Pa6.Click OK7.Edit the Outlet Boundary Condition8.On the Boundary Details tab, set the Relative Pressure to 300,000 Pa9.Click OKMost cavitation solutions should be performed by turning cavitation on and then successively lowering the system pressure over several runs to more

27、gradually induce cavitation. To speed up this workshop, a sudden change in pressure is introduced. Note that this approach may not be suitable for modelling some industrial cases.第17页/共23页第十七页，编辑于星期五：十三点 五十四分。Physics Modifications1.Edit Solver Control2.Set the Max. Iterations to 1503.Set the Residua

28、l Target to 1e-44.Click OK5.Close CFX-Pre and save the project6.In the Project Schematic, drag cell A3 onto cell B3The non-cavitating solution will be used as the initial guess for the cavitating solution7.Double-click Solution for the Cavitation systemIn the Solver Manager note that the initial con

29、ditions have been provided from the project schematic8.Click Start Run第18页/共23页第十八页，编辑于星期五：十三点 五十四分。Cavitation SolutionThere is a significant spike in residuals, in part due to the outlet pressure difference, but also due to the fact that the absolute pressure is low enough to induce cavitation.1.Wh

30、en the run completes, close the Solver Manager and return to the Project Schematic2.Save the project3.Double-click Results for the Cavitation project to openCFD-Post第19页/共23页第十九页，编辑于星期五：十三点 五十四分。Post-processing1.If it is not enabled, turn on visibility for the Wireframe and turn off visibility for a

31、ny User Locations and Plots2.Create an XY Plane at Z = 0.01 m3.Colour 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, which is a strong hint that some cavitation has occurred4.Change the Colour Variable to Water Vapour.Volume Fraction5.Change the Colour Map to Blue to White第20页/共23页第二十页，编辑于星期五：十三点 五十四分。Post-processing1.Turn off visibility for Plane 12.Create a Volume using the Isovolume method3.Set the Variable to Water