and to the following students who assisted in the creation of the Fluid Dynamics tutorials:

Transcription

1 Fluid Dynamics CAx Tutorial: Channel Flow Basic Tutorial # 4 Deryl O. Snyder C. Greg Jensen Brigham Young University Provo, UT Special thanks to: PACE, Fluent, UGS Solutions, Altair Engineering; and to the following students who assisted in the creation of the Fluid Dynamics tutorials: Leslie Tanner, Cole Yarrington, Curtis Rands, Curtis Memory, and Stephen McQuay.

2

3 2D Curved Flow In this tutorial, GAMBIT will be used to create and mesh the flow field geometry for the problem. Once this is complete, FLUENT will be used to solve for the pressure field everywhere in the domain and plot the pressure distribution across the pipe. This tutorial will provide experience in solving 2D flows and creating plots of the results. The methods expressed in these tutorials represent just one approach to modeling, constraining and solving 2D problems. Our goal is the education of students in the use of CAx tools for modeling, constraining and solving fluids application problems. Other techniques and methods will be used and introduced in subsequent tutorials. Water flows around the vertical two-dimensional bend with circular streamlines and constant velocity as shown below. If the pressure is 40 kpa at point (1), determine the pressure at points (2) and (3). Assume that the velocity profile is uniform as indicated. 3

4 Creating Geometry Begin the problem by creating geometry in Gambit. Start Gambit by either typing gambit at the command prompt (Unix or Windows) or clicking on the Gambit icon (Windows). The Gambit standard display should appear. Meshes are generated in Gambit by following left to right the menu icons located in the top right of the display window. The 2-D geometry will consist of two 90 arcs with lines connecting the ends. Create a node which will be used to define the center of curvature for the two arcs. Geometry > Vertex > Create Vertex Enter the Vertex at (0,6,0) as shown: Select Apply and Close. 4

5 Geometry > Edge > Create Real Circular Arc Note: Icons with a red arrow have a pull down menu. The arc button is located in the edges pull down menu. To activate the pull down menu select the icon with MB3. Buttons are then selected with MB1. Select the far right radio button Enter 6 for the radius, 225 and 315 for the angles. Select the center button. Select the vertex by holding the shift button and clicking MB1 over the vertex. Repeat for another arc of radius 4. Channel Flow Creating Geometry Now draw two lines to connect the arcs. Geometry > Edge > Create Edge Create lines to connect the arcs by shift selecting both end points and selecting Apply. Repeat for the other side of the channel. 5

6 Creating Geometry Next, create a face from the edges just created. Geometry > Face > Wireframe Shift select all four edges and click Apply. The edges should now be colored blue to indicate that the face has been created. If problems are encountered in creating the geometry, the geometry can be loaded from the file Bend_Geometry.dbs. 6

7 Meshing Geometry The geometry has now been created. The next step is to generate the mesh. First the edges must be meshed. Mesh > Edge > Mesh Edges Shift Select the left straight edge and the right straight edge. Change the pull-down menu to Interval count and enter 30. Click Apply. Repeat this procedure for the upper and lower walls. The screen should now look like this: Next mesh the face. Mesh > Face > Mesh faces Shift Select any edge of the geometry to select the face. Make sure the Element menu is set to Quad, Type is set to Map and then select Apply. The screen should look like this: If problems are encountered in meshing geometry, the meshed geometry can be loaded from the file Bend_Meshed.dbs. 7

8 Boundary Conditions Now define the boundary conditions for the problem. Since Fluent version 6 is going to be used, select Solver > Fluent5/6 from the pull-down menu across the top of the window. Operation > Zones > Specify Boundary Types Change the pull-down menu at the bottom to edges. This allows for selection of individual edges. Select the top and bottom edges. Name them walls and click Apply. Select the left straight edge, change the type pull-down menu to Velocity-Inlet, name it inlet and click Apply. Select the right straight edge, change the type pull-down menu to Outflow, name it outlet and click Apply. Now the geometry is ready to be exported. From the file pull-down menu, select File>export>mesh Select a location for the *.msh file and Accept. make sure to select the "export 2-D (X-Y) Mesh" radio button. Save and exit from Gambit. 8

9 If problems are encountered in specifying boundary conditions, the completed mesh with boundary conditions specified can be loaded from the file Bend_Complete.dbs. Channel Flow Starting in Fluent Open Fluent from the Desktop or Start menu. Select 2D Select Run The following window should appear. This is the FLUENT user interface. Most tasks are completed using the menus across the top. The menus are designed to guide you through the analysis in an orderly fashion, going from top to bottom through each menu, and left to right across the menu bar. Text commands can also be used in the command window. 9

10 Defining the Problem Start by importing the mesh created in Gambit. File > Read > Case A browse window should appear. Locate the *.msh file and select OK. FLUENT will read the mesh you created. If there are problems reading the mesh, return to the beginning of the tutorial and make sure you follow the steps carefully. If there are no problems the command window should state done. Now check the grid for errors. Grid > Check Any errors will be listed, otherwise the command window should again state done. 10

11 Defining the Problem Because the problem statement assumes a constant velocity profile across the channel, the flow will be modeled as inviscid. Define > Models > Viscous Select the Inviscid radio button and then OK. Now the fluid properties must be specified. The fluid properties are found by selecting: Define > Materials Select database... to browse through the FLUENT library of materials. Scroll down and select water-liquid (h2o<l>). Select Copy to copy these material properties into the current problem. Select Close on the Database Materials windows, followed by Close on the Materials window. Note: it is very important to click on the copy button. The fluid properties will not be loaded if the copy button is not selected. 11

12 Defining the Problem In order to set gravitational conditions as specified in the problem, select: Define > Operating Conditions Click on the Gravity radio button. Set the Operating pressure to be Pa and Gravity to be m/s 2 in the y direction. Click Ok. Now the velocity condition at the inlet and fluid type must be specified. Define > Boundary Conditions Select fluid under zones menu. Select fluid from the type menu. Click on set... From the Material Name pull down menu select the fluid that was previously added to the list, namely water-liquid (h2o<l>). Select Ok. 12

13 Defining the Problem Now to set the inlet conditions, select the inlet on the left, then select Set... Set the velocity magnitude to 10m/s. Select Ok and close the Boundary Conditions window. Specify which discretization functions will be used to calculate the solution. Solve > Controls > Solution In the Solution Control dialogue box, set the under-relaxation coefficients to Pressure = 0.9 Density = 1 Body Forces = 1 Momentum = 0.7 Also, change the Discretization functions to: PRESTO! SIMPLEC 2nd order upwind Click Ok. 13

14 Defining the Problem Next, the solution must be initialized. To do this: Solve > Initialize > Initialize From the Compute From pull-down menu, select the name given to the inlet wall. Select Init then close. Note: Once again, if initialize is not selected before close is, the case will remain un-initialized. By default, while trying to converge to a solution, FLUENT will stop iterating at a prescribed convergence threshold. Since the residuals will be plotted and analyzed graphically, it is not necessary to have FLU- ENT do this. To change this select: Solve > Monitors > Residual Place a check mark next to the Plot option using MB1. Make a new window by incrementing Window from 0 to 1. Deselect all of the check convergence boxes. Select Ok. 14

15 Defining the Problem In order to view the pressure field including the hydrostatic pressure, create a "Custom Field Function Define > Custom Field Function Create the function defined as follows: absolute-pressure - density * 9.81 * y Select absolute-pressure from the pulldown menu as shown: Click Select. Select the subtract sign. Select density from the pull-down menu and click select Select the multiplication (X) sign Enter 9.81 on the calculator pad Select the multiplication sign Select the y-coordinate as follows: First Pull-down menu: Grid Second Pull-down menu: Y-Coordinate Rename the function Press in the new function name box. Click Define and Close. 15

16 Defining the Problem In order to view pressure at discrete points, the points of interest must be created. Surface > Point... Create three points by entering the coordinate values and giving the point a name. If the bottom point surface creation fails, use a value slightly above zero (y=.0001), as shown. Create two points located at the middle (y=1) and top of the channel (y=2), respectively. Now set up monitors for these points under: Solve > Monitors > Surface... Set up three separate monitors (one for each point). Rename the monitors. Check the Print box for all three monitors. Choose Iteration from the Every pulldown menu. Select Define for the first monitor. Choose the point to be monitored from the Surfaces scroll menu. Change Report type to Sum. Verify that the correct Custom Field Function chosen from the Report of menu. Click Ok. Repeat for the remaining two points. Now, while iterating, there will be a column of pressure values displayed in the prompt window for each point. 16

17 Solving the Problem The problem is now ready to be solved. Select: Solve > Iterate Set the number of iterations to 100 and click Iterate. When iterations have completed close the iterate window. Note: It is preferable to have a view of the residuals handy so that they can be visually monitored., as shown. 17

18 Analyzing the Results Notice that the residuals have dropped by 6 to 7 orders of magnitude and have leveled out. This means that the solution has converged. To visually inspect the solutions, select Display > Contours From the pull-down menus select Pressure and select Display. The Pressure Distribution should look like this: 18

19 Analyzing the Results Now, since the pressure along the z-axis is desired, create a line along which to plot pressure vs. position by selecting: Surface > Line/Rake Enter the values as follows to define a line: x0 = 0 y0 = 0 x1 = 0 y1 = 2 Name the line centerline. Click create then close. Display the line in the display window by highlighting centerline in the Grid Display window, and clicking display. It should appear as shown: 19

20 Analyzing the Results Now plot the user-defined function by selecting: Plot > XY Plot From the pull down menu, select: Custom Field Functions... Select the line that was created: Change the plot direction as shown: Select Plot. The plot should look like this: If problems are encountered in setting up this problem in fluent, the solved problem can be read in as a Case and Data from the file Bend.cas. 20

21 Analytical Solution The analytical solution for the pressure along the vertical line from (1) to (3) is derived from ã dy dn p = n ñv R 2 Where γ is the specific weight of the fluid and ρ is the density. Substituting the geometry conditions for this problem and integrating yields P = P1 γy ρv At point (2), y=1m, and P 2 = 12.0kPa. At point (3), y=2m, and P 3 = -20.1kPa. The values predicted by Fluent are: P 2 = 13507kPa P 3 = kPa 2 6 ln 6 y which are in both in error by 13% and 9% respectively. The plot below shows a comparison of the analytical and CFD results Fluent Analytical 20.0 P (kpa) y(m) 21