Module B-Turbulent Pipe Flowdocx：模块b-turbulent管flowdocx.docxVIP

Module B: Turbulent Pipe FlowSummaryProblem StatementGeometry Creation Mesh Creation. Problem SetupSolution. Results. Post Processing.Validation. Structured vs. Unstructured Mesh Summary:The turbulent pipe flow learning module has three main objectives. First the user learns how to model a simple pipe in 2D under axisymmetric considerations. Then meshing the model is showcased as it relates to turbulent flowthe user learns how to apply bias to the meshing. Second proper problem setup is introduced in ANSYS FLUENT which involves setting the initial conditions and boundary conditions, checking for convergence and obtaining data. Third the user learns how to properly validate the obtained data in order to make sure the data is correct and makes sense. Validation is extremely important because if the user input the wrong parameters and specifications, the FLUENT output is also going to be incorrect. Extensive analysis has been perfomed on the obtained data for the turbulent pipe flow. It has been observed that while refining the structured mesh will not have a significant impact on the results it is important for that mesh to be structured otherwise erroneous results will be obtained. It has also been documented that more accurate results are obtained for a k-e turbulent model with near-wall treatment specified as enhanced wall treatment as opposed to standard wall functions. Turublent flow is validated by comparing with experimental data, i.e. skin friction, velocity profile and entry length.The important steps taken in creating the biased mesh, setting up the problem properly and obtaining meaningful validation can then be used as a basis for solving more complicated flow problems. Problem Statement:VinletCenter Line A typical pipe with given parameters: =1.0 kgm3; Vinlet=1ms; =2*10-5kgm*sD=0.2mL=8mFig. B.1Wall If we analyze a small element from the pipe, that element will have a rectangular shape. Since we are dealing with an axisymmetric flow the problem can be further simplified by focusing only on the radius of the shape.OutletVinletD/2Center LineLFig. B.2 The type of flow can be determined by calculating the Reynolds number:Re=*Vinlet*D (B.1)Re=1.0 kgm3*1ms*0.2 m(2*10-5)kgm*s=10 000 Recall that for flow in a round pipe, the flow is laminar if the Reynolds number is less than approximately 2100; the flow is transitional if the Reynolds number is between 2100 and 4000 and it is fully turbulent if Re is greater than 4000. Based on the given parameters the flow that is to be analyzed is fully turbulent. The flow will be analyzed by using Ansys Fluent, however first the geometry and the corresponding grid must be built. That will be done in Ansys Workbench. Afterwards the obtained results will be validated in order to make sure they make sense. Geometry Creation: Open ANSYS Workbench and start a new project. Since the flow is to be analyzed in Fluent, drag the Fluid Flow (Fluent) Analysis System to the project schematic. Since we are dealing with a 2d geometry, right click on Geometry and select Properties. Under Advanced Geometry Options for Analysis Type select 2d.Fig. B.3 Right click on geometry and select new geometry. Keep the default units of meters. From the Tree Outline select xy plane, then click the x-axis in the triad visible in the lower right corner in the graphics window.Fig. B.4 Select sketching from the Tree Outline. Then select Rectangle from the Draw options. In the graphics window place the cursor at the origin. The letter P should be visible meaning that point is fixed at the origin. Drag the pencil in the positive x and y directions thus creating the rectangle.Fig. B.5 Next the rectangles dimensions will be specified. Select Dimensions from the Sketching Toolboxes. Retain the default of General. In the Graphics Window, click on any of the two horizontal edges. By moving the pencil away from the edge and clicking once a ruler should be created. Then the horizontal dimension can be edited in the Details View, Dimensions. Set the horizontal dimension to 8 meters. Do the same for the vertical dimension and set it equal to 0.1 meters (we will analyze the flow as axisymmetric).Fig. B.6 You can zoom on selected portion of the geometry by selecting box zoom and by selecting pan the shape can be dragged around the screen. Click on Modeling under Sketching Toolboxes. Under the XY Plane select the created sketch and then choose Surfaces from Sketches from under Concept. Click apply in the Base Objects under Details of SurfaceSk. Fig. B.7 Finally select Generate to create the body. You can then exit the Design Modeler which will automatically save the created geometry. The check mark now visible next to geometry in the project schematic in workbench indicates no problems are detected and we can proceed with the mesh creation.Fig. B.8Mesh Creation: Double click on Mesh from the Fluid Flow System in the project schematic. Keep the Meshing Options defaults. Verify metric units are used (meters, kilograms, Newtons, etc). That can be done by selecting units. Select Mesh in the Outline. In Details of Mesh, under Sizing, select Off for Use Advanced Size Functions. This is necessary since we are manually going to specify the elements size and mesh type. Select Mesh Control, then Mapped Face Meshing. Select the face of the body (the rectangle should turn green) and click apply. By doing so opposite ends will correspond with each other.Fig. B.9 Under Mesh Control, select Sizing. Select the edge cube and select both horizontal edges by holding Ctrl. Click apply.Edge CubeSelect both edges.Fig. B.10 Under Type select Number of Divisions. Enter 100 divisions. Next to Behavior choose Hard. This is to overwrite the sizing function used by the ANSYS mesher. One hundred divisions are created in the axial direction.Fig. B.11 The mesh size for the two vertical edges is to be specified next. Select Sizing under Mesh Control. Select the left vertical edge (you can use pan to move the rectangle). Make sure the edge cube is turned on. Click Apply under Details of Sizing. Select Number of Divisions next to Type and enter 30 divisions. Since turbulence is heavily influenced by the presence of walls we would like the mesh to be denser as we get closer to the wall (upper horizontal edge). Hence a bias is needed. Zoom in to the left vertical edge. Select the 2nd bias type and enter a bias factor of 10. Make sure the elements get smaller as the wall is approached.Fig. B.12 Repeat the process for the other vertical edge. You can zoom out by selecting Zoom and while holding the left mouse button move the mouse diagonally leftwards. Then by selecting pan find the needed vertical edge. Again select Sizing from Mesh Control. Apply the right vertical edge and select 30 as the number of divisions. The bias factor is to be 10 as well but this time select the 1st bias type. It was required to specify the mesh size for the vertical edges individually since by default had the bias been specified for the two vertical edges selected together, the bias type would not match on the opposite ends.Turbulent flow analyzed by using k-e model, which is primarily valid away from walls therefore adjustments need to be made for the model to be accurate near walls. Hence a bias is required to provide more mesh near the wall.Fig. B.13 Next the zones are to be named. Select the upper horizontal edge. Right click and select Create Named Selections. Type Wall. Similarly type Inlet for the left vertical edge, Outlet for the right one, and Center Line for the bottom horizontal edge. It is necessary to specify the zones since the boundary conditions will be applied for those named zones in Fluent.Fig.B.14 Finally click on Update. The mesh should look like depicted in Fig. B.15. Fig. B.15 depicts a structured (mesh consisting of rectangles exhibiting a pronounced pattern) mesh of size 100X30-thirty divisions in the radial direction and 100 divisions in the axial one. You can now exit Meshing (it will be automatically saved). In the project schematic, next to meshing a check mark should appear signaling no issues were found. Double click on Setup. Fig. B.15Problem Setup: In the Fluent Launcher keep the default except for Options. There select Double Precision in order to increase accuracy of the solution, however more memory will be used.Fig B.16 Once in Fluent, in Problem SetupGeneral, select check. The mesh will be checked by Fluent and any errors will be reported. In Volume Statistics make sure the minimum volume is positive since if it is not, computation will not be possible. Fig.B.17 In GeneralSolver, keep the defaults except for 2D space. There choose axisymmetric. In General- Scale verify the dimensions of the mesh (x=8m, y=0.1m) and that meters are used for the length.Fig.B.18 In GeneralDisplay verify all the named surfaces are present, select all of them.Fig.B.19Problem SetupModels: Make sure the energy equation is off since we are dealing with incompressible flow (constant density) and we are not interested in temperature effects. Under viscous select the k-e (2eqns) model since the flow is turbulent (Re=10 000). Under Near-Wall Treatment select Enhanced Wall Treatment in order to obtain a more accurate solution. This will be verified later on when the flow is analyzed with Standard Wall Functions Near-Wall Treatment.Fig.B.20Problem SetupMaterials: Double click on air. Enter 1.0 kgm3 for the density and 2*10-5kgm*s for the viscosity. Enter change/createthe entered data overwrites the pre-existing material information.Fig.B.21 If the material is saved not overwriting the pre-existing air material but is saved as a separate material (ex. the data is saved as material named custom) an extra step is required to make sure the model is analyzed using the proper material properties. In Problem SetupCell Zone Conditions, double click the surface_body zone. Under Material Name make sure the proper material is selectedin the given example the material named custom should be selected. Press OK.Fig B.22Problem SetupBoundary Conditions:Table B.1 Verify and if needed change the zone types as depicted in Table B.1ZoneTypecenter_lineAxisinletVelocity-inletInterior-surface bodyInterioroutletPressure-outletwallWall Double Click on inlet. Enter 1m/s for the velocity magnitude (given value). Under Turbulence, select Intensity and Hydraulic Diameter. Specify 1% for Turbulent Intensity and 0.2meters for the Hydraulic Diameter.Fig B.23Problem SetupBoundary Conditions: Double click on outlet. Verify the gauge pressure is set to 0 (since the difference between the absolute pressure at the outlet, 1atm, and the operating pressure, 1 atm, equals to 0 which is the gauge pressure at the outlet).Fig.B.24 Verify in the Operating Conditions that the Operating Pressure is set to 101, 325 Pa which equals 1 atm.Fig.B.25Problem SetupReference Values: Set the reference values to be computed from the inlet as this is required in order to obtain certain flow solutions such as the skin friction and Y+ values.Fig.B.26Solution:Solution-Solution Methods: Under Partial Discretization make sure the Momentum, Turbulent Kinetic Energy and the Turbulent Dissipation Rate Gradients are set to 2nd Order Upwind. The 2nd order upwind provides better accuracy while the 1st order upwind provides a more robust convergence. Fig.B.27SolutionMonitors: Double click on Residuals. Make sure the Print to Console and Plot options are checked. In Equations set the absolute criteria to 1e-06 for all 5 equations. Residuals provide a measure of how well the current solution satisfies the discrete form of each of the governing equations.Fig.B.28SolutionInitialization: The input data and conditions must be initialized in order for a solution to be obtained. Select Compute from Inlet and press Initialize.Fig.B.29SolutionRun Calculation: The next important step before a solution is obtained is to check for convergence. The governing equations must converge to a limiting value meaning a point comes where they are no longer changing. Enter one hundred for the number of iterations and press Calculate. However 100 iterations are not enough to obtain convergence for a turbulent model of mesh size 100X30. Hence enter 500 for the number of iterations thus restarting the calculations without having to initialize again. The five hundred iterations to be performed are done after the already calculated 100. In the message that appears stating the Setting have changed, you can simply keep the first choice and press ok. Fluent stops once the solution has converged.Fig.B.30Results:Velocity Vectors: A typical pipe with the corresponding velocity profile for turbulent flow is illustrated in Fig.B.31Fig.B.31 The velocity profile can be displayed by going to ResultsGraphics and Animations and double clicking Vectors under GraphicsFig.B.32. Refer to Appendix AResults about colormap and vectors manipulation. Fig.B.33 showcases the fully developed velocity vectors.Fig.B.32OutletAxisFig.B.33Fully Developed Velocity Vectors near the Pipes Outlet XY Plots will be performed for the Y+values, centerline velocity in the axial direction, the skin friction coefficient, the fully developed velocity profile in the radial direction and the pressure drop. The solutions will then be validated against the theoretical data in order to make sure they are correct and make sense. Finally by improving the mesh we will try to obtain a more accurate solution. Y+values:o In ResultsPlots select XY Plot. Double click it. Make sure Position on X axis is selected as well as Node Values. In Plot Direction make sure x=1 and y=0 (x will thus become the abscissa or horizontal coordinate). Select Turbulence from under Y Axis Function and choose Wall Yplus. Select the wall surface. Click on Plot.Y+ is a non-dimensional wall distance for a wall-bounded flow, defined as y+=u*y (B.2)where y is the distance to the nearest wall u* is the friction velocity at the nearest wall, is the local kinematic viscosity.Y+ is calculated from the reference values specified, , Vinlet Fig.B.34Fig.B.35 The graph can be saved as a picture by selecting Save Picture under File. The different saving options are explained when Help is pressed. The graph can be manipulated by going back to the XY Plot and selecting curves, the markers can be replaced by a line with a user chosen color and weight.Fig.B.36 The graph can be further enhanced by manipulating the y-axis values. By selecting Axes, in the number format the type can be changed from exponential to float. Make sure to click apply after a change has been made for a particular axis. The graph produced as a result is shown in Fig.B.37:Fig.B.37Fig.B.38The plot can be saved by clicking on Write to File in the Solution XY Plot window. Press Write afterwards and save the plot as a .xy file. The .xy file can be then opened in Excel where dimensional analysis for validation purposes can be performed. This will be demonstrated later. Fig.B.39ResultsCenterline Velocity PlotIn ResultsPlots, XY Plot, in the Y-axis function select Velocity and Axial Velocity. Deselect the wall surface by clicking it again and select the centerline surface. Click Plot. Fig.B.40Fig.B.41 The title of the plot can be changed by double clicking on the default text in the lower left corner. Save the plot by selecting the Write to File and clicking Write. It can be seen the fully developed region starts at around x=4m.ResultsSkin Friction Coefficient: In the XY Plot window select Wall Fluxes under Y-axis Function and specify Skin Friction Coefficient. Select the Wall Surface. Fig.B.42Fig.B.43 Skin friction, Cf is the drag on the plate produced by the boundary layer due to viscous stresses which are developed at the wall. It also reffered as the Fanning friction factor. Cfw.5*ref*vref2 (B.3) Results FD Velocity Profile: In the Solution XY Plot deselect Position on X Axis and select Position on Y axis since we are to plot the velocity profile in the radial direction. In Plot Direction set x=0 and y=1. Under X Axis Function select Velocity and specify Axial Velocity. Since we are interested in the fully developed profile select the outlet surface. Save the created plot.Fig.B.44Fig.B.45Post Processing: A crucial step in the post processing step of fluid flow analysis is the validation. It needs to be determined whether or not the results obtained from Fluent make sense and if they do how accurate are they. To do this the mesh will be refined and the data obtained from it and the mesh already used will be compared to theoretical solutions.Post ProcessingMesh Refinement: In the Project Schematic in Workbench right click on Fluid Flow (Fluent) and select Duplicate. An exact replica including the solution will be created in th