给大佬的培训fluent

1、Workshop 05 Turbulent Flow Past a Backwards Facing StepWorkshop Description:Flow over a backwards facing step is a standard test case for turbulence models. We will see how to set up and solve turbulent flow problems in Fluent and learn to use CFD-Post and Workbench to compare the results from diffe

2、rent turbulence models with each other and with experimental data. We will also examine how the results are affected by boundary conditionsLearning Aims:The workshop covers many aspects of turbulent flow modeling in Fluent including specifying models and near wall treatments, checking y+, selecting

3、boundary conditions, comparison with experimental results and comparison of results obtained with different turbulence modelsLearning Objectives:To understand how to set up and solve turbulent flows in Fluent using different models and near wall treatmentsTo understand how to post process y+ in Flue

4、ntTo understand the importance of realistic boundary conditionsTo understand how to compare results with data using CFD-Post and easily perform results comparisons using WorkbenchIIntroductionIntroductionModel SetupSolvingPost-ProcessingSummarySimulation to be performedThe task is to simulate flow o

5、ver a backwards facing stepThe simulation is being performed to determine:How the results from different turbulence models compare with one another and with experimental resultsCan the models predict the reattachment point downstream of the step?Flow separates at the step and reattaches some distanc

6、e downstreamIntroductionModel SetupSolvingPost-ProcessingSummaryStart a new workbench session.Drag a Fluent component system onto the projectRight-click on Setup, and select Import Fluent Case, and BrowseIn the pop-up window, change the filter (bottom-right) from case to “Fluent Mesh File”Browse to

7、and select the file“driver.msh.gz” Click OK on the Fluent Launcher screenLoading the mesh and starting FluentIntroductionModel SetupSolvingPost-ProcessingSummaryDisplay MeshDisplay the mesh and then zoom in on the mesh near the bottom wall downstream of the stepIntroductionModel SetupSolvingPost-Pro

8、cessingSummaryIt is intended for the simulation to resolve the viscous sublayer with the mesh (no wall functions), which requires a very fine near wall mesh to get y+ 1.Later in the workshop, we will evaluate whether this has been achieved.The distance corresponding to y+ = 1 can be estimated as des

9、cribed in Lecture 7.Activate ModelsOpen the Viscous Models panel and select the Realizable k-epsilon with Enhanced Wall TreatmentWhen using any k-epsilon model, the Enhanced Wall Treatment is the only viscous sublayer resolving near wall treatment.Later on we will calculate the flow with the SST k-o

10、mega model and compare results.IntroductionModel SetupSolvingPost-ProcessingSummaryDefine MaterialsKeep the default values for the density and viscosity of airIntroductionModel SetupSolvingPost-ProcessingSummaryThe inlet boundary conditions are shown belowThe default backflow settings for the outlet

11、 are sufficient for this problem, so no entries are required for the pressure outlet boundaryBoundary ConditionsTo begin with, uniform profiles will be used. In a later step, the flow will be puted using fully developed flow profiles for velocity and turbulence at the inlet.IntroductionModel SetupSo

12、lvingPost-ProcessingSummarySolution MethodsIn the Solution Methods panel, change the option for Pressure-Velocity Coupling from SIMPLE to Coupled and select Pseudo Transient near the bottom of the panelChange pressure to PRESTO! In many cases, the solution will converge in fewer iterations using Cou

13、pled plus the Pseudo Transient method.PRESTO! is often a better choice for structured hexahedral or quadrilateral meshes such as has been created for this problem.IntroductionModel SetupSolvingPost-ProcessingSummaryIntroductionModel SetupSolvingPost-ProcessingSummaryMonitorsIn Monitors, press Create

14、. for a Surface MonitorEnter wall-shear-monfor the nameCheck the box to Plot and set the window number to 2Choose Area-Weighted Average for the report typeChoose Wall Shear Stress for the field variableSelect bottom_wall as the surfaceThe Wall Shear Stress on the wall downstream of the step is the q

15、uantity of interest in this simulation, so it is natural to track it with a solution monitor.IntroductionModel SetupSolvingPost-ProcessingSummaryMonitorsCreate another surface monitorEnter turb-out-mon for the nameCheck the box next to plot and immediately below that set Window to 3Select Area-Weigh

16、ted Average for the report typeSelect Turbulent Viscosity Ratio for the field variableSelect outlet_p in the list of surfacesThe solution for turbulence model variables can change very slowly in regions far downstream from inlets. Because of this they are often good to use for solution monitors. Tur

17、bulent viscosity ratio is selected here because it includes contributions from both the turbulent kinetic energy and the turbulent dissipation rate, meaning both fields have to converge before the monitor stops changing.Calculate the SolutionInitialize the solution using hybrid initialization, save

18、the project, and then go to the Run Calculation panel and ask for 100 iterationsThe residuals converge in a small number of iterations, but the monitors do not definitively indicate that the solution has stopped changingIntroductionModel SetupSolvingPost-ProcessingSummaryContinue the CalculationSet

19、the continuity residual criterion to 1e-6Use the TUI command /solve/monitors/surface/clear-data to clear the solution monitorsIn the Run Calculation panel, request 100 more iterationsChoose Use settings for current calculation onlyThere is no significance to 1e-6. It is just desired to select a low

20、value so the iterations do not stop prematurely. Additional iterations will be performed and convergence will be judged by whether the surface moonitors are still changing.This step is not strictly necessary but it helps to make the y-axis range in the monitor plots tighter, thus making it easier to

21、 see changes in the monitored variable.IntroductionModel SetupSolvingPost-ProcessingSummaryJudging ConvergenceAfter an additional 100 iterations, neither surface monitor is changing and the residuals have all reached very low levelsTogether, these conditions indicate the solution is convergedSave th

22、e project before moving onIntroductionModel SetupSolvingPost-ProcessingSummaryQuick Post-Processing: Wall YplusPlot y+ along the bottom wallWall Yplus is near the bottom of the list under turbulence variables. For 2D problems such as this, xy plots are an ideal way to check the y+ distribution. Node

23、 values have been unselected because although y+ is calculated at wall faces, its value is stored for post-processing in the wall adjacent cells.These values are a little bit higher than ideal. We will see later how it affects comparison with experiment, and it would be highly mended to do a mesh se

24、nsitivity study if this were an actual study as opposed to a workshop exercise.IntroductionModel SetupSolvingPost-ProcessingSummaryQuick Post-Processing: VectorsDisplay velocity vectors and zoom in on the step regionThe vectors show the recirculation zone behind the step and the subsequent reattachm

25、ent of the flow. Some adjustment of the Scale and Skip setting in the panel is probably required for optimal viewing of the vectors.IntroductionModel SetupSolvingPost-ProcessingSummaryChange the turbulence modelClose Fluent, return to Workbench and save the projectIn the project schematic, right cli

26、ck on the Fluent cell and rename it as RKERight click again on the Fluent cell and select DuplicateRename the duplicate cell to SST and Edit the setup block in this cellIntroductionModel SetupSolvingPost-ProcessingSummarySelect SST ModelIn the Viscous Models panel, select the SST model as shownRepea

27、t the steps performed in Slides 12, 13 and 14In Fluent, the turbulence models that use omega do not require the selection of a near wall treatment. This is because the near wall treatment that is used is a y+ insensitive method that automatically behaves either as a viscous sublayer resolving treatm

28、ent or as a wall function depending on how fine or coarse the near wall mesh is.IntroductionModel SetupSolvingPost-ProcessingSummarySST: Convergence and Post-processingConvergence is very good both for this problem with both SST and Realizable k-epsilonYplus is qualitatively similar. Next we will us

29、e CFD Post to make a more quantitative comparisonSave the project, exit Fluent and return to the Project SchematicIntroductionModel SetupSolvingPost-ProcessingSummaryPost-Processing in CFD-PostFrom Component Systems drag a Results object into the Project SchematicLeft click on the Solution cell for

30、RKE (A3) and without releasing the mouse, drag the pointer on top of Results (C2)Repeat the previous step with the Solution cell for SST (B3). The Project Schematic should appear as to the right. Double click on Results to start CFD-PostIntroductionModel SetupSolvingPost-ProcessingSummaryVelocity Ve

31、ctorsClick on Insert and choose VectorsSelect symmetry 1 for the location and change the reduction factor to 2Click on the Symbol tab and enter a value of 0.5 for Symbol Size (not shown)Zoom in on the region just behind the stepThe velocity fields here are very similar. In the next step a more quant

32、itative comparison will be made using the shear stress on the wall downstream of the step.Use these icons to synchronize views and the visibility of objects.For 2D models, CFD-Post extrudes the geometry a small distance in the 3rd direction. The resulting symmetry planes are used for results display

33、.IntroductionModel SetupSolvingPost-ProcessingSummaryChanging the reduction factor to 2 means that only every other vector will be displayed, which makes the vectors easier to see.ExpressionsComparisons of results are often made using geometrical coordinates normalized by the step height. This can b

34、e done with the help of variables and expressionsClick the Expressions tab, then right click and select NewName the expression step height and define the expression as shown (below)It is also possible to type 0.0127 m in the definition field. Defining the expression as shown here will allow it to up

35、date automatically if the step height were to be changed, for instance in a parametric study.Right click in the details field for context menus to add functions and locations without having to type them manually.IntroductionModel SetupSolvingPost-ProcessingSummaryExpressionsCreate a second expressio

36、n for the dimensionless x-coordinate named xh expression as shown belowIntroductionModel SetupSolvingPost-ProcessingSummaryVariablesIn order to use the previous expression to plot the wall shear stress, a variable needs to be createdClick the Variables tab, right click on User Defined, select New an

37、d create a variable named XhIntroductionModel SetupSolvingPost-ProcessingSummaryPolylineA polyline defined by the intersection of the symmetry boundary and the bottom wall is required in order to plot the wall shear stressThere is more than one way to define this polyline, but the Boundary Intersect

38、ion method is probably the most convenient in this case and its use ensures the polyline definition would remain consistent if changes were made upstream in the project workflow.IntroductionModel SetupSolvingPost-ProcessingSummaryCreate a ChartSelect Insert ChartIn the Details panel, select the poly

39、line created in the previous step in the Data Series tabSelect Xh for the X Axis variable and Wall Shear X for the Y AxisWall Shear X is used instead of Wall Shear because the location where it changes sign identifies the flow reattachment point.IntroductionModel SetupSolvingPost-ProcessingSummaryWa

40、ll Shear Stress Comparison The resulting plot appears in the Chart ViewerThe reattachment point is identified where the shear stress changes sign. Also the positive values very close to the step indicate the presence of a small secondary recirculation zone. This can also be seen by zooming in on the

41、 vector plot and increasing the symbol size.The size and strength of the recirculation zone predicted by either model is remarkably similar. However, because of the proximity of the inlet to the step, the use of uniform inlet profiles is questionable. That will be explored later on in the workshop.

42、IntroductionModel SetupSolvingPost-ProcessingSummaryAdd External Data to ChartRight click in the data field in the chart details and select NewName the new series Exp., select File, navigate to the workshop files directory, change Files of type to All Files (*) and select cf_ds.xyIntroductionModel S

43、etupSolvingPost-ProcessingSummaryPlot External DataSelect the Line Display tab in the chart details and change the display options as shown belowThe data appears on the chart as seen to the rightThe external data is from the experiment of Driver and Seegmiller. Agreement between the CFD results and

44、the data is not very good, however the uniform inlet boundary conditions do not correspond to those seen experimentally in the same location.In the following steps, fully developed velocity and turbulence profiles will be applied at the inlet in order to mimic the experimental conditions.Introductio

45、nModel SetupSolvingPost-ProcessingSummaryChanging the Inlet Boundary ConditionRight click on the RKE cell in the Project Schematic and select DuplicateName the newly created Fluent object RKE Profile, right click on the Setup cell and select EditIntroductionModel SetupSolvingPost-ProcessingSummaryAd

46、ding ProfilesNavigate to Define Profiles, select Read in the Profiles panel, navigate to the workshop files directory and select the file fOpen the boundary conditions panel for the Velocity Inlet and use the drop down arrows apply the profiles as shown to the rightBe sure to change the

47、turbulence specification method to K and EpsilonFully developed profiles are produced by running an auxiliary calculation in a small domain with periodic boundary conditions. The files from this calculation are available in the workshop files folderIntroductionModel SetupSolvingPost-ProcessingSummar

48、yRunning the CalculationInitialize the flow with hybrid initialization and perform the calculation exactly as in Slides 12-14Good convergence behavior also with the new boundary conditionsNote that by creating a duplicate of the original Fluent object, it was not necessary to redefine any of the sol

49、ution monitors, material properties or solver settings. Only the boundary conditions needed to be changed.IntroductionModel SetupSolvingPost-ProcessingSummaryRun SST with Profile Boundary ConditionsIn the Project Schematic, create a duplicate of the SST Fluent object and name it SST ProfileClick Edi

50、t in the Setup cell of the new object, go to Define Profiles and read the profile fApply the profile at the inlet boundary Initialize the solution with Hybrid Initialization and run the calculation using the same steps described in Slides 12-14IntroductionModel SetupSolvingPost-Processin

51、gSummaryDuplicating the Results ObjectRight click on the Results object in the Project Schematic and select DuplicateThe original calculations with uniform boundary conditions are connected to this cell. Right click on each of the connections and select DeleteIntroductionModel SetupSolvingPost-Proce

52、ssingSummaryExamining the New ResultsLeft click on the Solution cell for RKE Profile(F3) and without releasing the mouse, drag the pointer on top of Results with Profiles (D2)Repeat with SST Profile so that the Project Schematic appears as shownThe labeling of the individual blocks A,B,C,D, may be d

53、ifferent in your caseDouble click on Results with Profiles to launch CFD-PostIntroductionModel SetupSolvingPost-ProcessingSummaryComparing Results with Profile BCsDouble click on Chart 1 in the Outline Tree to open the chartThe chart is automatically updated with the new resultsDiscussion:Use of realistic, fully developed velocity and turbulence profiles at the inlet greatly improves the agreement between the results and the experiment. These results do not represent a formal validation study. In particul