ansys_cfd流体分析实例

Example on using commercial software“ICEM CFD 5.1”Flow around a circular cylinderY.F.LinTwo Dimensional problemsFlow around a circular cylinderProblem DescriptionAir flows across a cylinder with the uniform velocity 0.003m/s in the wind tunnel. The length of the wind tunnel (fluid domain) has 25m long and 10 m height. The diameter of cylinder is 1m.Wall (SideA)InletOutlet5DCylinderWall (SideB)Fluid domain5D20DAssumption and Boundary Conditions:1. 2 dimensional problems2. Steady state condition3. The uniform flow velocity4. No Heat transfer5. Neglect the gravitational force6. Constant air densityPre-processing stageIn this stage, we implement the “ICEM CFD” to perform the pre-processing work. The basic steps as follow:1. Establish geometry model2. Block the parts3. Generation the O grid4. Mesh the model and check quality of mesh5. Extrude the mesh6. Reset the BCs (boundary conditions)7. Output to CFX5.7.1 Creating Geometry1. Open ICEM CFDDouble Click the “ICEM CFD” Icon, afterwards, you can see the interface of the ICEM CFD.Open FileNew Project: Set the name with “cylinder_2d”, and Click “Save”2. Creating Geometry:A. PointsClick button “Create Point” and then click button “Explicit Coordinates”Set the points in Cartesian coordinate system(X, Y, Z) with ( X=0, Y=0, Z=0 ) respectively.Click “Apply” button and see the screen: a point is created A tree widget can be seen at left of the screen (A) and (B) The same method creates other points:X=0; Y=0.5, -0.5 X=-5; Y=5, -5X=20; Y=5, -5 Y=0; X=0.5,-0.5 B. Draw line (curve)First of all see the tree widget, open ModelGeometryPoints by right buttonSelect Show Point Names and you can see the name of each point like the figure showed.Now you can create curves Click button “Create/Modify Curve” Click button “Create Curve” Note: the left corner of the black screen: Select locations with left button, middle=done, right=cancelSelect points by using left button of the mouse.Change the name of the Part with “INLET”: Select PONITS.05 and POINTS.06 with left button (A),And draw a line with middle button “done” (B) and the INLET part is created in the tree widget.The same steps draw the curves named “OUTLET, SIDEA, SIDEB” with the POINTS.07and POINTS.08, POINTS.06 and POINTS.07, POINTS.05 and POINTS.08 respectively.We will see the line and the tree widget Draw the cylinderClick button “Circle or arc from Center point and 2 points on plane”. Set the Part with name “CYLINDER”Click button and select points “POINTS.00, POINTS.01, POINTS.03” with left button respectively (A). Draw the cylinder by middle button (B).See tree widget:Close Points nameUse button to fit the window.Set the body and material. Click button “Create Body”Choose button “Material Point” and select “Selected surfaces” in the “By Topology” menu.Change the name of the part with “FLUID”; open the Show Point Name of the tree widget and use select POINTS.06 and POINTS.08.The same way change the part name with “CYLINDER” and select POINTS.01 and POINTS.02.Close Show Point Name and open the tree widget:Open the bodies and you can seeAt last, open the FileGeometrySave Geometry AsGive it the name with “cylinder_2d”. Click “save”. Now we begin to block the model. Click button “Create Block”See the first one , choose the part with “FLUID”, from the pull down menu select “FLUID”And set the Initialize Blocks type with “2D Planar” Click “Apply” button. We will see that the colors of figure are changed. From (A) to (B)See the tree widget: ModelBlockingThen create some assistant points with button “Create Point”Y=0 X=-0.45,-0.4,-0.35,-0.3,-0.25,-0.2,-0.15,-0.1,-0.5, 0.5, 0.1, 0.15, 0.2, 0.25, 0.3, 0.35, 0.4, 0.45X=0 Y=-0.45,-0.4,-0.35,-0.3,-0.25,-0.2,-0.15,-0.1,-0.5, 0.5, 0.1, 0.15, 0.2, 0.25, 0.3, 0.35, 0.4, 0.45Now begin to block the region Click button “Split Block” Then select button “Split Block” See the split method, select “Prescribed point”Use the put down menu to select the Prescribed point, Use the button firstly select the Edge “INLET” and secondly select the Point “POINTS.03”.We will see the block line in the vertical direction of the INLET.Zoom the fiure.The same way we draw other block lines.From the “POINTS.01 to POINTS.04” See the tree widgetSelect the “Blocking” and select “Index Control” ModelBlocking: Index Control (using right button of the mouse)We can see at the right corner of the screenBy using button and we set I min=2 and see the figure The same way we set I max =3 , J min=2 , J max=3And the screen shown that The same way block again from “POINTS.00, POINTS.09 to POINTS.44”:(A)(B)(C) After block.See the tree widget: ModelPartsVORFN :using the right button select “Add to Part”. Click button “Blocking Material”, Add Blocks to PartUsing select blocking regions and we can see Zoom the block regions (A).Select the blocks in the cylinder or attached the cylinder (B)(C). Using the middle button to set it OK, and you can see blow (D). Click button “Associate” Select the associate edge to curve “Associate Edge to Curve” buttonUsing the choose the edge and curveChoosing edge:Select curves: Middle button:Set O grid Click button “Split Block” Click “Ogird Block” buttonSelect the See the tree widget: Open ModelPartsVORFNOpen the VORFN (A)Using button to select in or attached the cylinder (B)(C)(D). Using middle button to click “Apply” (E)Close “VORFN” from the tree widget (F) Click the “Reset”(G)Mesh the edges Click button “Set Curve Mesh Size” Using button to select Curve(s): Choose Method with “Element count” Set the Number with 100 and click Apply.See the tree: close the ModelGeometrypoints, and the ModelBlockingedgesUsing right button to select ModelGeometryCurves: Curve Node Spacing (by using right button)The same way set the “INLET” and “OUTLET” with number 100, the “SIDEA” and “SIDEB” with number 250. Click button “Pre-Mesh Params”Choose Blocking Pre-Mesh ParamsClick button “Update Sizes” and keep default, Then click ApplySee tree open ModelBlockingPre_Mesh: Project faces (by using right button)And we will see a menu Click Yes.Now we will see the mesh of the model.Zoom it see the local part Close GeomeryPoints and curves, and BlockingEdges.Then open FileMeshLoad from BlockingOpen FileMeshSave Mesh As: and set the name with “cylinder_2d”Open FileBlockingSave Blocking As: Save block with the name “cylinder_2d”Check the quality of the mesh Click button “Display Mesh Quality” Click ApplyWe can see no negatives mesh.Extrude meshClick button “Extrude Mesh” Use to select Elements:Method 1Click button “Select items in a part” and a menu appears:Click “All” and “Accept”Method 2 Put the left button and drag it to select all the regions (A)(C). Click middle button to accept (B)Give the New volume part name “FLUID2D”, new side part name “SIDE”, new top par name “TOP”And set the Spacing typespacing with “0.1”, then ApplySo the mesh change a height 0.1 in the Z direction (D)Box Zoom Click button “Shaded Full Display”(E)(F)Check the quality of the extrude meshSee the tree widget:Close top “TOP” (B)Close “FLUID” (C)Set the new boundary conditionsSee the tree widget:ModelParts: Create Part (by using the right button) Click “Create Part by Selection” button From the pull down menu of the Part: select the “CYLINDER”Using and left button drag the region Using middle button accepts it, so a new CYLINDER boundary condition has been set (C).The same way set the INLET, OUTLET, SIDEA and SIDEB boundary conditions.INLET The Whole Boundary ConditionsSee the tree widget:Open ModelPartsFLUID(B)Open ModelPartsTOP(C)Six kinds of patternsClick FileMeshSave Mesh AsAnd save the new mesh with name “cylinder_2d_extrude”.Output the mesh file to CFXClick button “Select solver” and choose “CFX-5” Click “Okay”Click button “Write input” Keep default and click “Done”Then the Domain selection appears Keep the Selected domains with “cylinder_2d_extrude.uns” and click “Done”.Now we will see the created files in working directions:From these files, we must note that only the file named “cfx5” can be inputted into CFX5.7.1The mesh is finished.Other examples: Example on using commercial software“CFX 5.7.1”Flow around a circular cylinderY.F.LinTwo Dimensional problemsFlow around a circular cylinderAfter established the geometry model, we begin to use CFX to solve this two dimensional case.Processing with CFX-5.7.11. Open CFXDouble click the “CFX” Icon, afterwards, you can see the interface of the CFX.There are three kinds of functions of the CFX:1. CFX-Pre 5.7.1 (set the relevant parameters).2. CFX-Solver 5.7.1 (solve the case by using established physical model)3. CFX-Post 5.7.1 (get the data and figures which we need)CFX-Pre step:1. Import the mesh file from ICEM CFD2. Simulation type3. Domain4. BCs (boundary conditions)5. Initial conditions6. Solver control7. Output file and monitor points8. Write “.def” file and simulationClick button “CFX-Pre 5.7.1” and run it.Establish a new simulationOpen FileNew Simulation: Select button “General” and give the file name with “cylinder_2d”. Click “Save”Now we can see the interface of the CFX-PreImport mesh fileSee the middle position of the screen, Click button “Import mesh” Open MeshDefinitionMesh Format: From the pull down menu select “ICEM CFD”, (see figure below) DefinitionFile: Click button “Browse”Find the working direction and select the file named “cfx5”, Then click “Open” button. And “OK” Note: no other files can be inputted in CFX5.7.1 Then the mesh file has been inputted into the CFX-Pre And the left window appears.All of these names were already defined by us in “ICEM CFD” Set the relevant parameters1. Define the simulation type: Click button “Define the Simulation Type” button.Note: the blue color note suggest we should set a domain.Then the simulation type appearsBasic SettingsOption: Select “Transient” Basic SettingsTime DurationOption: From the pull down menu select Total Time.Basic SettingsTime DurationTotal Time: Set with 42000s.Basic SettingsTime StepsOption: From the pull down menu select Timesteps.Basic SettingsTime StepsTimesteps: Set with 1s.Initial TimeOption: From the pull down menu select Autorratic.Then click Apply and Ok2. Create a domain: Click button “Create a Domain” . Set the name with “ cylinder2d” and click OkSee figure below: the color of the domain changed into green, and the window “Edit Domain” appears. General OptionsBasic SettingsLocation:From the pull down menu select “FLUID2D”Then click “Apply” buttonFluid ModelsHeat Transfer ModelOption: Keep by default.Fluid ModelsHeat Transfer ModelFluid Temperature: Set the temperature with 25c.Fluid ModelsTurbulence ModelOption: Set it with “None(Laminar). Click OK 3. Set boundary condtions: Click button “Create a Boundary Condition”Set INLET boundary condition Set the Name with “INLET” and click OK Basic SettingsBoundary Type: From the pull down menu select INLET.Boundary DetailsFlow RegimeOption: Select Subsonic.Boundary DetailsMass And MomentumOption: Select Normal Speed.Boundary DetailsMass And MomentumNormal Speed: Set it with 0.003 m/sClick OkThe right figure shows us that the INLET boundary condition has been set.Set OUTLET boundary conditionSet the Name with “OUTLET” and click OKBasic SettingsBoundary Type: OutletBasic SettingsLocation: From the pull down menu select OUTLET.Boundary DetailsFlow RegimeOption: Select Subsonic.Boundary DetailsMass And MomentumOption: Select Average Static Pressure.Boundary DetailsMass And MomentumRelative Pressure: Set with 0 Pa. Boundary DetailsPressure AveragingOption: Keep by defaultThen click OK The right figure shows us that the OUTLET boundary condition has been set.Set Wall boundary conditions Set the Name with “SIDEA” and click OK Basic SettingsBoundary Type: Wall.Basic SettingsLocation: From the pull down menu select SIDEA.Boundary DetailsWall Influence On FlowOption: Set with No Slip.Then click OkThe right figure shows us that the Wall boundary condition has been set (SIDEA).The same way set SIDEB The right figure shows us that the Wall boundary condition has been set.(SIDEB).Set the CYLINDER with “Wall”Set the Name with “CYLINDER” and click OKThe right figure shows us that the Wall boundary condition has been set (CYLINDER).Set “Fluid” and “Top” with symmetry boundary conditionsSet the Name with “SYM” and click OKBasic SettingsBoundary Type: Symmetry.Basic SettingsLocation: Click button, then hold “Ctrl” button of the keyboard and use the left button of mouse to select FLUID and TOP. Click OKThen Click Apply and OkThe right figure shows us that the Symmetry boundary condition has been set (FLUID and TOP).4. Define the initial conditions Click button “Define the Global Initial Conditions”Global SettingsFrame TypeFrame Type: From the pull down menu select Stationary.Global SettingsInitial ConditionsVelocity Type: From the pull down menu select Cartesian.Global Settings Cartesian Velocity ComponentsOption: Automatic with Value.Global Settings Cartesian Velocity ComponentsU: Set it with 0.003m/s.Keep other options by default and click Apply, OK5. Define the solver control Click button “Define the Solver Control Criteria” Basic SettingsAdvection SchemeOption: High Resolution.Basic SettingsTransients SchemeOption: From the pull down menu select Second Order Backward Euler.Basic SettingsConvergence ControlMax.Iter.Per.Timestep: set it with 50.Basic SettingsConvergence CriteriaResidual Type: From the pull down menu select RMS.Basic SettingsConvergence CriteriaResidual Target: Set it with 1e-7Then click “Ok”.6. Create output files and monitor points Click button “Create Output Files and Monitor Points”ResultsOption: From the pull down menu select Full.ResultsFile Compression Level: Default.Monitor: Use left button of mouse select Monitor Options.Then click Apply and Ok. Note: After this work, open: FileSave simulation: and save the file which named “cylinder_2d.cfx”7. Save files Click button “Write a Solver File”Click OK and run the CFX-Solver automatically.CFX-Solver 5.7.1We can also run the CFX-Solver by click button “CFX-Solver 5.7.1” Open FileDefine RunAnd select the file which we need, see figure below:The interface of the CFX-SolverRun DefinitionDefinition File: Use button to find the file named “cylinder_2d.def” in working directions and select it.Then click Start Run button. We can use button to stop the simulation, and a small pop-up window appears. Click OK, and the simulation can be stopped.If we want to continue run the case, click button CFX-Post 5.7.1Click button “CFX-Post 5.7.1”, afterwards, we can see the interface of the CFX-Post. Open FileLoad ResultsAssuming we have gotten some results. Select the last one named “cylinder_2d_017.res” and click “Open”Then the model appears in the screen.See the left figure, all the regions are set at the tree widget. We can select the objects which we need, such as CYLINDER, INLET, SYM, etc. Also we can use button to edit them.