fluent 学习资料 Laminar Pipe Flow.doc

Problem Specification1. Create Geometry in GAMBIT2. Mesh Geometry in GAMBIT3. Specify Boundary Types in GAMBIT4. Set Up Problem in FLUENT5. Solve!6. Analyze Results7. Refine MeshProblem 1Problem 2Laminar Pipe FlowProblem SpecificationConsider fluid flowing through a circular pipe of contant cross-section. The pipe diameter D=0.2 m and length L=8 m. The inlet velocity Vin=1 m/ s. Consider the velocity to be constant over the inlet cross-section. The fluid exhausts into the ambient atmosphere which is at a pressure of 1 atm. Take density =1 kg/ m3 and coefficient of viscosity = 2 x 10-3 kg/(ms). The Reynolds number Re based on the pipe diameter is where Vavg is the average velocity at the inlet, which is 1m/s in this case. Solve this problem using FLUENT. Plot the centerline velocity, wall skin-friction coefficient, and velocity profile at the outlet. Validate your results. Note: The values used for the inlet velocity and flow properties are chosen for convenience rather than to reflect reality. The key parameter value to focus on is the Reynolds no. Preliminary AnalysisWe expect the viscous boundary layer to grow along the pipe starting at the inlet. It will eventually grow to fill the pipe completely (provided that the pipe is long enough). When this happens, the flow becomes fully-developed and there is no variation of the velocity profile in the axial direction, x (see figure below). One can obtain a closed-form solution to the governing equations in the fully-developed region. You should have seen this in the Introduction to Fluid Mechanics course. We will compare the numerical results in the fully-developed region with the corresponding analytical results. So its a good idea for you to go back to your textbook in the Intro course and review the fully-developed flow analysis. What are the values of centerline velocity and friction factor you expect in the fully-developed region based on the analytical solution? What is the solution for the velocity profile? Well create the geometry and mesh in GAMBIT which is the preprocessor for FLUENT, and then read the mesh into FLUENT and solve for the flow solution. Go to Step 1: Create Geometry in GAMBITStep 1: Create Geometry in GAMBITStrategy for Creating GeometryIn order to create the rectangle, we will first create the vertices at the four corners. Well then join adjacent vertices by straight lines to form the edges of the rectangle. Lastly, well create a face corresponding to the area enclosed by the edges. In Step 2, well mesh the face i.e. the rectangle. Note that in 3D problems, youll have to form a volume from faces. So the hierarchy of geometric objects in GAMBIT is vertices - edges - faces - volumes.Create a Working DirectoryCreate a folder called pipe in a convenient location. Well use this as the working folder in which files created during the session will be stored. Note for ACCEL computer lab users: Each user gets his/her own 100 MB of disk space under S: at ACCEL. You can put your files in S: and itll be accessible from any computer. This is where you should put files that you want to keep and access later on. Start GAMBITStart your command prompt. Start Run In Windows NT/2000/XP: Type cmd and press enter.In Windows 95/98/ME: Type command and press enter. Navigate your way to your working folder. For example, if you created a folder named fluent on drive S: in Windows, type cd S:fluent at the command prompt and press Enter. Start GAMBIT by typing gambit -id pipe at the command prompt and pressing Enter. If this doesnt work, try typing the full pathname to the GAMBIT executable: c:fluent.incntbinntx86gambit -id pipe This brings up the GAMBIT interface and tells GAMBIT to use pipe as the default prefix for all files created during the session. In Windows, the Exceed X-server starts up before the GAMBIT interface comes up. Exceed is a third-party application needed to render the interface in Windows (GAMBIT was originally developed under Unix). To make best use of screen real estate, move the windows and resize them so that you approximate this screen arrangement. This way you can read instructions in the browser window and implement them in GAMBIT. You can resize the text in the browser window to your taste and comfort:In Internet Explorer: Menubar View Text Size, then choose the appropriate font size.In Netscape: Menubar View Increase Font or Menubar View Decrease Font.The GAMBIT Interface consists of the following: Main Menu Bar: Note that the job name pipe appears after ID: in the title bar of the Utility Menu. Operation Toolpad:Well more or less work our way across the Operation Toolpad as we go through the solution steps. Notice that as each of the top buttons is selected, a different sub-pad appears. The Geometry sub-pad is shown in the above snaphot. Global Control Toolpad:The Global Control Toolpad has options such as Fit to Screen and Undo that are very handy during the course of geometry and mesh creation. GAMBIT Graphics:This is the window where the graphical results of operations are displayed. GAMBIT Description Panel:The Description Panel contains descriptions of buttons or objects that the mouse is pointing to. Move your mouse over some buttons and notice the corresponding text in the Description Panel. GAMBIT Transcript Window:This is the window to which output from GAMBIT commands is written and which provides feedback on the actions taken by GAMBIT as you perform operations. If, at some point, you are not sure you clicked the right button or entered a value correctly, this is where to look to figure out what you just did. You can click on the arrow button in the upper right hand corner to make the Transcript window full-sized. You can click on the arrow again to return the window to its original size. Go ahead, give this a try.Select SolverSpecify that the mesh to be created is for use with FLUENT 6.0:Main Menu Solver FLUENT 5/6Verify this has been done by looking in the Transcript Window where you should see:The boundary types that youll be able to select in the third step depends on the solver selected.We can assume that the flow is axisymmetric. The problem domain is:where r and x are the radial and axial coordinates, respectively.Strategy for creating geometryWe will put the origin of the coordinate system at the lower left corner of the rectangle. The coordinates of the corners are shown in the figure below:We will first create four vertices at the four corners and join adjacent vertices to get the edges of the rectangle. We will then form a face that covers the area of the rectangle.Create VerticesFind the buttons described below by pointing the mouse at each of the buttons and reading the Description Window.Operation Toolpad Geometry Command Button Vertex Command Button Create Vertex Notice that the Create Vertex button has already been selected by default. After you select a button under a sub-pad, it becomes the default when you go to a different sub-pad and then come back to the sub-pad.Create the vertex at the lower-left corner of the rectangle:Next to x:, enter value 0. Next to y:, enter value 0. Next to z:, enter value 0 (these values should be defaults). Click Apply. This creates the vertex (0,0,0) which is displayed in the graphics window. In the Transcript window, GAMBIT reports that it Created vertex: vertex.1. The vertices are numbered vertex.1, vertex.2 etc. in the order in which they are created. Repeat this process to create three more vertices:Vertex 2: (0,0.1,0)Vertex 3: (8,0.1,0)Vertex 4: (8,0,0)Note that for a 2D problem, the z-coordinate can always be left to the default value of 0. Operation Toolpad Global Control Fit to Window Button This fits the four vertices of the rectangle we have created to the size of the Graphics Window. (Click picture for larger image)Create EdgesWell now connect appropriate pairs of vertices to form edges. To select any entity in GAMBIT, hold down the Shift key and click on the entity. Operation Toolpad Geometry Command Button Edge Command Button Create Edge Select two vertices that make up an edge of this rectangle by holding down the Shift button and clicking on the corresponding vertices. As each vertex is picked, it will appear red in the Graphics Window. Then let go of the Shift button. We can check the selected vertices by clicking on the up-arrow next to Vertices:. This will bring up a window containing the vertices that have been selected. Vertices can be moved from the Available and Picked lists by selecting them and then pressing the left or right arrow buttons. After the correct vertices have been selected, click Close, then click Apply in the Create Straight Edge window. Repeat this process to create a rectangle. (Click picture for larger image) Create FaceOperation Toolpad Geometry Command Button Face Command Button Form Face To form a face out of the area enclosed by the four lines, we need to select the four ledges that enclose this area. This can be done by holding down the Shift key, clicking on each line (notice that the currently selected line appears red), and then releasing the Shift key after all four lines have been selected. Alternatively, an easier way to do this would be to click on the up arrow next to edges:This will bring up the Edge List window. Click on All- to select all of the edges at once. Click Close.Click Apply to create the face.Go to Step 2: Mesh Geometry in GAMBIT Step 2: Mesh Geometry in GAMBITWell now create a mesh on the rectangular face with 100 divisions in the axial direction and 5 divisions in the radial direction. Well first mesh the four edges and then the face. The desired grid spacing is specified through the edge mesh. Mesh EdgesOperation Toolpad Mesh Command Button Edge Command Button Mesh Edges Shift-click or bring up the Edge List window and select both the vertical lines. If this is difficult, one can zoom in on an edge by holding down the Ctrl button, clicking and dragging the mouse to specify an area to zoom in on, and releasing the Ctrl button. To return to the main view, click on the Global Control Toolpad Fit to Window Button again. Once a vertical edge has been selected, select Interval Count from the drop down box that says Interval Size in the Mesh Edges Window. Then, in the box to the left of this combo box, enter 5 for the interval count. Click Apply. Nodes appear on the edges showing that they are divided into 5. (Click picture for larger image) Repeat the same process for the horizontal edges, but with an interval count of 100. Now that the edges are meshed, we are ready to create a 2-D mesh for the face. Mesh FaceOperation Toolpad Mesh Command Button Face Command Button Mesh Faces Shift left-click on the face or use the up arrow next to Faces to select the face. Click Apply. (Click picture for larger image) Go to Step 3: Specify Boundary Types in GAMBIT Step 3: Specify Boundary Types in GAMBITCreate Boundary TypesWell next set the boundary types in GAMBIT. The left edge is the inlet of the pipe, the right edge the outlet, the top edge the wall, and the bottom edge the axis. Operation Toolpad Zones Command Button Specify Boundary Types Command Button This will bring up the Specify Boundary Types window on the Operation Panel. We will first specify that the left edge is the inlet. Under Entity:, pick Edges so that GAMBIT knows we want to pick an edge (face is default). Now select the left edge by Shift-clicking on it. The selected edge should appear in the yellow box next to the Edges box you just worked with as well as the Label/Type list right under the Edges box. Next to Name:, enter inlet. For Type:, select VELOCITY_INLET. Click Apply. You should see the new entry appear under Name/Type box near the top of the window. Repeat this process for the other three edges according to the following table: Edge PositionNameTypeLeftinletVELOCITY_INLETRightoutletPRESSURE_OUTLETTopwallWALLBottomcenterlineAXISYou should have the following edges in the Name/Type list when finished:Save and ExportMain Menu File Save Main Menu File Export Mesh. Type in pipe.msh for the File Name:. Select Export 2d Mesh since this is a 2 dimensional mesh. Click Accept. Check pipe.msh has been created in your working directory. Go to Step 4: Set Up Problem in FLUENT Step 4: Set Up Problem in FLUENTLaunch Fluent 6.0Start Programs Fluent Inc FLUENT 6.0 Select 2ddp from the list of options and click Run. The 2ddp option is used to select the 2-dimensional, double-precision solver. In the double-precision solver, each floating point number is represented using 64 bits in contrast to the single-precision solver which uses 32 bits. The extra bits increase not only the precision but also the range of magnitudes that can be represented. The downside of using double precision is that it requires more memory. Import GridMain Menu File Read Case.Navigate to the working directory and select the pipe.msh file. This is the mesh file that was created using the preprocessor GAMBIT in the previous step. FLUENT reports the mesh statistics as it reads in the mesh:Check the number of nodes, faces (of different types) and cells. There are 500 quadrilateral cells in this case. This is what we expect since we used 5 divisions in the radial direction and 100 divisions in the axial direction while generating the grid. So the total number of cells is 5*100 = 500.Also, take a look under zones. We can see the four zones inlet, outlet, wall, and centerline that we defined in GAMBIT. Check and Display GridFirst, we check the grid to make sure that there are no errors. Main Menu Grid Check Any errors in the grid would be reported at this time. Check the output and make sure that there are no errors reported. Check the grid size: Main Menu Grid Info Size The following statistics should appear: Display the grid: Main Menu Display Grid. Make sure all 5 items under Surfaces is selected. Then click Display. The graphics window opens and the grid is displayed in it. You can now click Close in the Grid Display menu to get back some desktop space. The graphics window will remain. Some of the operations available in the graphics window are: Translation: The grid can be translated in any direction by holding down the Left Mouse Button and then moving the mouse in the desired direction. Zoom In: Hold down the Middle Mouse Button and drag a box from the Upper Left Hand Corner to the Lower Right Hand Corner over the area you want to zoom in on. Zoom Out: Hold down the Middle Mouse Button and drag a box anywhere from the Lower Right Hand Corner to the Upper Left Hand Corner. Use these operations to zoom into the grid to obtain the view shown below. Note: The zooming operations cannot be performed without a middle mouse button. (Click picture for larger image) You can also look at specific parts of the grid by choosing the boundaries you wish to view under Surfaces (click to select and click again to deselect a specific boundary). Click Display again when you have selected your boundaries. For example, the wall, outlet, and centerline boundaries have been selected in the following view: These options will display the graph: (Click picture for larger image) For convenience, the button next to Surfaces selects all of the boundaries while the deselects all of the boundaries at once. Close the Grid Display Window when you are done. Define Solver PropertiesMain Menu Define Models Solver Choose Axisymmetric under Space. Well use the defaults of segregated solver, implicit formulation, steady flow and absolute velocity formulation. Click OK. Main Menu Define Models Viscous Laminar flow is the default. So we dont need to change anything in this menu. Click Cancel. Main Menu Define Models Energy For incompressible flow, the energy equation is decoupled from the continuity and momentum equations. We need to solve the energy equation only if we are interested in determining the temperature distribution. We will not deal with temperature in this example. So leave the Energy Equation unselected and click Cancel to exit the menu. Define Material PropertiesMain Menu Define Materials. Change Density to 1.0 and Viscosity to 2e-3. These are the values that we specified under Problem Specification. Well take both as constant. Click Change/Create. Define Operating ConditionsMain Menu Define Operating Conditions. For all flows, FLUENT uses gauge pressure internally. Any time an absolute pressure is needed, it is generated by adding the operating pressure to the gauge pressure. Well use the default value of 1 atm (101,325 Pa) as the Operating Pressure. Click Cancel to leave the default in place. Define Boundary ConditionsWell now set the value of the velocity at the inlet and pressure at the outlet.Main Menu Define Boundary Conditions. We note here that the four types of boundaries we defined are specified as zones on the left side of the Boundary Conditions Window. The centerline zone should be selected by default. Make sure it is, then make sure the Type of this boundary is selected as axis and click Set. Notice that there is nothing to set for the axis. Click OK. Move down the list and select inlet under Zone. Note that FLUENT indicates that the Type of this boundary is velocity-inlet. Recall that the boundary type for the inlet was set in GAMBIT. If necessary, we can change the boundary type set previously in GAMBIT