Using a Single Rotating Reference Frame

Tutorial 9. Using a Single Rotating Reference Frame Introduction This tutorial considers the flow within a 2D, axisymmetric, co-rotating disk cavity system. Understanding the behavior of such flows is important in the design of secondary air passages for turbine disk cooling. This tutorial demonstrates how to do the following: Set up a 2D axisymmetric model with swirl, using a rotating reference frame. Use the standard k-ɛ and RNG k-ɛ turbulence models with the enhanced near-wall treatment. Calculate a solution using the pressure-based solver. Display velocity vectors and contours of pressure. Set up and display XY plots of radial velocity and wall y + distribution. Restart the solver from an existing solution. Prerequisites This tutorial is written with the assumption that you have completed Tutorial 1, and that you are familiar with the ANSYS FLUENT navigation pane and menu structure. Some steps in the setup and solution procedure will not be shown explicitly. Problem Description The problem to be considered is shown schematically in Figure 9.1. This case is similar to a disk cavity configuration that was extensively studied by Pincombe [1]. Air enters the cavity between two co-rotating disks. The disks are 88.6 cm in diameter and the air enters at 1.146 m/s through a circular bore 8.86 cm in diameter. The disks, which are 6.2 cm apart, are spinning at 71.08 rpm, and the air enters with no swirl. As the flow is diverted radially, the rotation of the disk has a significant effect on the viscous flow developing along the surface of the disk. Release 12.0 c ANSYS, Inc. March 12, 2009 9-1

Outflow 44.3 cm Rotating Disk Rotating Disk 6.2 cm Inflow 4.43 cm 71.08 rpm Figure 9.1: Problem Specification As noted by Pincombe [1], there are two nondimensional parameters that characterize this type of disk cavity flow: the volume flow rate coefficient, C w, and the rotational Reynolds number, Re φ. These parameters are defined as follows: C w = Q ν r out (9.1) Re φ = Ωr2 out ν (9.2) where Q is the volumetric flow rate, Ω is the rotational speed, ν is the kinematic viscosity, and r out is the outer radius of the disks. Here, you will consider a case for which C w = 1092 and Re φ = 10 5. 9-2 Release 12.0 c ANSYS, Inc. March 12, 2009

Setup and Solution Preparation 1. Download single_rotating.zip from the User Services Center to your working folder (as described in Tutorial 1). 2. Unzip single_rotating.zip. The file disk.msh can be found in the single rotating folder created after unzipping the file. 3. Use FLUENT Launcher to start the 2D version of ANSYS FLUENT. For more information about FLUENT Launcher, see Section 1.1.2 in the separate User s Guide. Note: The Display Options are enabled by default. Therefore, once you read in the mesh, it will be displayed in the embedded graphics window. Step 1: Mesh 1. Read the mesh file (disk.msh). File Read Mesh... As ANSYS FLUENT reads the mesh file, it will report its progress in the console. Step 2: General Settings General 1. Check the mesh. General Check ANSYS FLUENT will perform various checks on the mesh and report the progress in the console. Make sure that the reported minimum volume is a positive number. 2. Examine the mesh (Figure 9.2). Extra: You can use the right mouse button to check which zone number corresponds to each boundary. If you click the right mouse button on one of the boundaries in the graphics window, information will be displayed in the ANSYS FLUENT console about the associated zone, including the name of the zone. This feature is especially useful when you have several zones of the same type and you want to distinguish between them quickly. Release 12.0 c ANSYS, Inc. March 12, 2009 9-3

Mesh FLUENT 12.0 (2d, dp, pbns, lam) Figure 9.2: Mesh Display for the Disk Cavity 3. Define new units for angular velocity and length. General Units... In the problem description, angular velocity and length are specified in rpm and cm, respectively, which is more convenient in this case. These are not the default units for these quantities. (a) Select angular-velocity from the Quantities list, and rpm in the Units list. (b) Select length from the Quantities list, and cm in the Units list. (c) Close the Set Units dialog box. 9-4 Release 12.0 c ANSYS, Inc. March 12, 2009

4. Specify the solver formulation to be used for the model calculation and enable the modeling of axisymmetric swirl. General (a) Retain the default selection of Pressure-Based in the Type list. (b) Retain the default selection of Absolute in the Velocity Formulation list. For a rotating reference frame, the absolute velocity formulation has some numerical advantages. (c) Select Axisymmetric Swirl in the 2D Space list. Release 12.0 c ANSYS, Inc. March 12, 2009 9-5

Step 3: Models Models 1. Enable the standard k-ɛ turbulence model with the enhanced near-wall treatment. Models Viscous Edit... (a) Select k-epsilon in the Model list. The Viscous Model dialog box will expand. (b) Retain the default selection of Standard in the k-epsilon Model list. (c) Select Enhanced Wall Treatment in the Near-Wall Treatment list. (d) Click OK to close the Viscous Model dialog box. The ability to calculate a swirl velocity permits the use of a 2D mesh, so the calculation is simpler and more economical to run. This is especially important for problems where the enhanced wall treatment is used. The near-wall flow field is resolved through the viscous sublayer and buffer zones (that is, the first mesh point away from the wall is placed at a y + of the order of 1). For details, see Section 4.12.4 in the separate Theory Guide. 9-6 Release 12.0 c ANSYS, Inc. March 12, 2009

Step 4: Materials Materials For the present analysis, you will model air as an incompressible fluid with a density of 1.225 kg/m 3 and a dynamic viscosity of 1.7894 10 5 kg/m-s. Since these are the default values, no change is required in the Create/Edit Materials dialog box. 1. Retain the default properties for air. Materials air Create/Edit... Extra: You can modify the fluid properties for air at any time or copy another material from the database. 2. Click Close to close the Create/Edit Materials dialog box. For details, see Chapter 8 in the separate User s Guide. Release 12.0 c ANSYS, Inc. March 12, 2009 9-7

Step 5: Cell Zone Conditions Cell Zone Conditions Set up the present problem using a rotating reference frame for the fluid. Then define the disk walls to rotate with the moving frame. 9-8 Release 12.0 c ANSYS, Inc. March 12, 2009

1. Define the rotating reference frame for the fluid zone (fluid-7). Cell Zone Conditions fluid-7 Edit... (a) Select Moving Reference Frame from the Motion Type drop-down list. (b) Enter 71.08 rpm for Speed in the Rotational Velocity group box. (c) Click OK to close the Fluid dialog box. Release 12.0 c ANSYS, Inc. March 12, 2009 9-9

Step 6: Boundary Conditions Boundary Conditions 9-10 Release 12.0 c ANSYS, Inc. March 12, 2009

1. Set the following conditions at the flow inlet (velocity-inlet-2). Boundary Conditions velocity-inlet-2 Edit... (a) Select Components from the Velocity Specification Method drop-down list. (b) Enter 1.146 m/s for Axial-Velocity. (c) Select Intensity and Hydraulic Diameter from the Specification Method dropdown list in the Turbulence group box. (d) Enter 2.6% for Turbulent Intensity. (e) Enter 8.86 cm for Hydraulic Diameter. (f) Click OK to close the Velocity Inlet dialog box. Release 12.0 c ANSYS, Inc. March 12, 2009 9-11

2. Set the following conditions at the flow outlet (pressure-outlet-3). Boundary Conditions pressure-outlet-3 Edit... (a) Retain the default selection of Normal to Boundary from the Backflow Direction Specification Method drop-down list. (b) Select Intensity and Viscosity Ratio from the Specification Method drop-down list in the Turbulence group box. (c) Enter 5% for Backflow Turbulent Intensity. (d) Retain the default value of 10 for Backflow Turbulent Viscosity Ratio. (e) Click OK to close the Pressure Outlet dialog box. Note: ANSYS FLUENT will use the backflow conditions only if the fluid is flowing into the computational domain through the outlet. Since backflow might occur at some point during the solution procedure, you should set reasonable backflow conditions to prevent convergence from being adversely affected. 9-12 Release 12.0 c ANSYS, Inc. March 12, 2009

3. Accept the default settings for the disk walls (wall-6). Boundary Conditions wall-6 Edit... (a) Click OK to close the Wall dialog box. Note: For a rotating reference frame, ANSYS FLUENT assumes by default that all walls rotate at the speed of the moving reference frame, and hence are moving with respect to the stationary (absolute) reference frame. To specify a nonrotating wall, you must specify a rotational speed of 0 in the absolute frame. Release 12.0 c ANSYS, Inc. March 12, 2009 9-13

Step 7: Solution Using the Standard k-ɛ Model 1. Set the solution parameters. Solution Methods (a) Retain the default selection of Least Squares Cell Based from the Gradient list in the Spatial Discretization group box. (b) Select PRESTO! from the Pressure drop-down list in the Spatial Discretization group box. The PRESTO! scheme is well suited for steep pressure gradients involved in rotating flows. It provides improved pressure interpolation in situations where large body forces or strong pressure variations are present as in swirling flows. (c) Select Second Order Upwind from the Momentum, Swirl Velocity, Turbulent Kinetic Energy, and Turbulent Dissipation Rate drop-down lists. Use the scroll bar to access the discretization schemes that are not initially visible in the task page. 9-14 Release 12.0 c ANSYS, Inc. March 12, 2009

2. Set the solution controls. Solution Controls (a) Retain the default values in the Under-Relaxation Factors group box. Note: For this problem, the default under-relaxation factors are satisfactory. However, if the solution diverges or the residuals display large oscillations, you may need to reduce the under-relaxation factors from their default values. For tips on how to adjust the under-relaxation parameters for different situations, see Section 26.3.2 in the separate User s Guide. Release 12.0 c ANSYS, Inc. March 12, 2009 9-15

3. Enable the plotting of residuals during the calculation. Monitors Residuals Edit... (a) Ensure that Plot is enabled in the Options group box. (b) Click OK to close the Residual Monitors dialog box. Note: For this calculation, the convergence tolerance on the continuity equation is kept at 0.001. Depending on the behavior of the solution, you can reduce this value if necessary. 9-16 Release 12.0 c ANSYS, Inc. March 12, 2009

4. Enable the plotting of mass flow rate at the flow exit. Monitors (Surface Monitors) Create... (a) Enable the Plot and Write options for surf-mon-1. Note: When the Write option is selected in the Surface Monitor dialog box,the mass flow rate history will be written to a file. If you do not enable thewrite option, the history information will be lost when you exit ANSYS FLUENT. (b) Select Mass Flow Rate from the Report Type drop-down list. (c) Select pressure-outlet-3 from the Surfaces selection list. (d) Click OK in the Surface Monitor dialog box to enable the monitor. Release 12.0 c ANSYS, Inc. March 12, 2009 9-17

5. Initialize the flow field using the boundary conditions set at velocity-inlet-2. Solution Initialization (a) Select velocity-inlet-2 from the Compute From drop-down list. (b) Click Initialize. 6. Save the case file (disk-ke.cas.gz). File Write Case... 9-18 Release 12.0 c ANSYS, Inc. March 12, 2009

7. Start the calculation by requesting 500 iterations. Run Calculation (a) Enter 500 for the Number of Iterations. (b) Click Calculate. Throughout the calculation, ANSYS FLUENT will report reversed flow at the exit. This is reasonable for the current case. The solution should be sufficiently converged after approximately 225 iterations. The mass flow rate history is shown in Figure 9.3. Figure 9.3: Mass Flow Rate History (k-ɛ Turbulence Model) Release 12.0 c ANSYS, Inc. March 12, 2009 9-19

8. Check the mass flux balance. Reports Fluxes Set Up...! Although the mass flow rate history indicates that the solution is converged, you should also check the net mass fluxes through the domain to ensure that mass is being conserved. (a) Select velocity-inlet-2 and pressure-outlet-3 from the Boundaries selection list. (b) Retain the default Mass Flow Rate option. (c) Click Compute and close the Flux Reports dialog box.! The net mass imbalance should be a small fraction (say, 0.5%) of the total flux through the system. If a significant imbalance occurs, you should decrease the residual tolerances by at least an order of magnitude and continue iterating. 9. Save the data file (disk-ke.dat.gz). File Write Data... Note: If you choose a file name that already exists in the current folder, ANSYS FLU- ENT will prompt you for confirmation to overwrite the file. 9-20 Release 12.0 c ANSYS, Inc. March 12, 2009

Step 8: Postprocessing for the Standard k-ɛ Solution 1. Display the velocity vectors. Graphics and Animations Vectors Set Up... (a) Enter 50 for Scale (b) Set Skip to 1. (c) Click the Vector Options... button to open the Vector Options dialog box. i. Disable Z Component. This allows you to examine only the non-swirling components. ii. Click Apply and close the Vector Options dialog box. Release 12.0 c ANSYS, Inc. March 12, 2009 9-21

(d) Click Display in the Vectors dialog box to plot the velocity vectors. A magnified view of the velocity field displaying a counter-clockwise circulation of the flow is shown in Figure 9.4. Figure 9.4: Magnified View of Velocity Vectors within the Disk Cavity (e) Close the Vectors dialog box. 2. Display filled contours of static pressure. Graphics and Animations Contours Set Up... 9-22 Release 12.0 c ANSYS, Inc. March 12, 2009

(a) Enable Filled in the Options group box. (b) Retain the selection of Pressure... and Static Pressure from the Contours of drop-down lists. (c) Click Display and close the Contours dialog box. The pressure contours are displayed in Figure 9.5. Notice the high pressure that occurs on the right disk near the hub due to the stagnation of the flow entering from the bore. Figure 9.5: Contours of Static Pressure for the Entire Disk Cavity 3. Create a constant y-coordinate line for postprocessing. Surface Iso-Surface... Release 12.0 c ANSYS, Inc. March 12, 2009 9-23

(a) Select Mesh... and Y-Coordinate from the Surface of Constant drop-down lists. (b) Click Compute to update the minimum and maximum values. (c) Enter 37 in the Iso-Values field. This is the radial position along which you will plot the radial velocity profile. (d) Enter y=37cm for the New Surface Name. (e) Click Create to create the isosurface. Note: The name you use for an isosurface can be any continuous string of characters (without spaces). (f) Close the Iso-Surface dialog box. 4. Plot the radial velocity distribution on the surface y=37cm. Plots XY Plot Set Up... (a) Select Velocity... and Radial Velocity from the Y Axis Function drop-down lists. (b) Select the y-coordinate line y=37cm from the Surfaces selection list. (c) Click Plot. Figure 9.6 shows a plot of the radial velocity distribution along y = 37 cm. 9-24 Release 12.0 c ANSYS, Inc. March 12, 2009

Figure 9.6: Radial Velocity Distribution Standard k-ɛ Solution (d) Enable Write to File in the Options group box to save the radial velocity profile. (e) Click the Write... button to open the Select File dialog box. i. Enter ke-data.xy in the XY File text entry box and click OK. 5. Plot the wall y+ distribution on the rotating disk wall along the radial direction (Figure 9.7). Plots XY Plot Set Up... (a) Disable Write to File in the Options group box. (b) Select Turbulence... and Wall Yplus from the Y Axis Function drop-down lists. Release 12.0 c ANSYS, Inc. March 12, 2009 9-25

(c) Deselect y=37cm and select wall-6 from the Surfaces selection list. (d) Enter 0 and 1 for X and Y respectively in the Plot Direction group box. (e) Click the Axes... button to open the Axes - Solution XY Plot dialog box. i. Retain the default selection of X from the Axis group box. ii. Disable Auto Range in the Options group box. iii. Retain the default value of 0 for Minimum and enter 43 for Maximum in the Range group box. iv. Click Apply and close the Axes - Solution XY Plot dialog box. (f) Click Plot in the Solution XY Plot dialog box. Figure 9.7 shows a plot of wall y+ distribution along wall-6. Figure 9.7: Wall Yplus Distribution on wall-6 Standard k-ɛ Solution 9-26 Release 12.0 c ANSYS, Inc. March 12, 2009

(g) Enable Write to File in the Options group box to save the wall y+ profile. (h) Click the Write... button to open the Select File dialog box. i. Enter ke-yplus.xy in the XY File text entry box and click OK. Note: Ideally, while using enhanced wall treatment, the wall y+ should be in the order of 1 (at least < 5) to resolve viscous sublayer. The plot justifies the applicability of enhanced wall treatment to the given mesh. (i) Close the Solution XY Plot dialog box. Step 9: Solution Using the RNG k-ɛ Model Recalculate the solution using the RNG k-ɛ turbulence model. 1. Enable the RNG k-ɛ turbulence model with the enhanced near-wall treatment. Models Viscous Edit... (a) Select RNG in the k-epsilon Model list. Release 12.0 c ANSYS, Inc. March 12, 2009 9-27

(b) Enable Differential Viscosity Model and Swirl Dominated Flow in the RNG Options group box. The differential viscosity model and swirl modification can provide better accuracy for swirling flows such as the disk cavity. For more information, see Section 4.4.2 in the separate Theory Guide. (c) Retain Enhanced Wall Treatment as the Near-Wall Treatment. (d) Click OK to close the Viscous Model dialog box. 2. Continue the calculation by requesting 200 iterations. Run Calculation The solution converges after approximately 105 additional iterations. 3. Save the case and data files (disk-rng.cas.gz and disk-rng.dat.gz). File Write Case & Data... Step 10: Postprocessing for the RNG k-ɛ Solution 1. Plot the radial velocity distribution for the RNG k-ɛ solution and compare it with the distribution for the standard k-ɛ solution. Plots XY Plot Set Up... (a) Enter 1 and 0 for X and Y respectively in the Plot Direction group box. (b) Select Velocity... and Radial Velocity from the Y Axis Function drop-down lists. (c) Select y=37cm and deselect wall-6 from the Surfaces selection list. 9-28 Release 12.0 c ANSYS, Inc. March 12, 2009

(d) Disable the Write to File option. (e) Click the Load File... button to load the k-ɛ data. i. Select the file ke-data.xy in the Select File dialog box. ii. Click OK. (f) Click the Axes... button to open the Axes - Solution XY Plot dialog box. i. Enable Auto Range in the Options group box. ii. Click Apply and close the Axes - Solution XY Plot dialog box. (g) Click the Curves... button to open the Curves - Solution XY Plot dialog box, where you will define a different curve symbol for the RNG k-ɛ data. i. Retain 0 for the Curve #. ii. Select x from the Symbol drop-down list. iii. Click Apply and close the Curves - Solution XY Plot dialog box. Release 12.0 c ANSYS, Inc. March 12, 2009 9-29

(h) Click Plot in the Solution XY Plot dialog box (Figure 9.8). Figure 9.8: Radial Velocity Distribution RNG k-ɛ and Standard k-ɛ Solutions The peak velocity predicted by the RNG k-ɛ solution is higher than that predicted by the k-ɛ solution.this is due to the less diffusive character of the RNG k-ɛ model. Adjust the range of the x axis to magnify the region of the peaks. (i) Click the Axes... button to open the Axes - Solution XY Plot dialog box, where you will specify the x-axis range. i. Disable Auto Range in the Options group box. ii. Retain the value of 0 for Minimum and enter 1 for Maximum in the Range dialog box. iii. Click Apply and close the Axes - Solution XY Plot dialog box. 9-30 Release 12.0 c ANSYS, Inc. March 12, 2009

(j) Click Plot. The difference between the peak values calculated by the two models is now more apparent. Figure 9.9: RNG k-ɛ and Standard k-ɛ Solutions (x = 0 cm to x = 1 cm) 2. Plot the wall y+ distribution on the rotating disk wall along the radial direction Figure 9.10. Plots XY Plot Set Up... Release 12.0 c ANSYS, Inc. March 12, 2009 9-31

(a) Select Turbulence... and Wall Yplus from the Y Axis Function drop-down lists. (b) Deselect y=37cm and select wall-6 from the Surfaces selection list. (c) Enter 0 and 1 for X and Y respectively in the Plot Direction group box. (d) Select any existing files that appear in the File Data selection list and click the Free Data button to remove the file. (e) Click the Load File... button to load the RNG k-ɛ data. i. Select the file ke-yplus.xy in the Select File dialog box. ii. Click OK. (f) Click the Axes... button to open the Axes - Solution XY Plot dialog box. i. Retain the default selection of X from the Axis group box. ii. Retain the default value of 0 for Minimum and enter 43 for Maximum in the Range group box. iii. Click Apply and close the Axes - Solution XY Plot dialog box. (g) Click Plot in the Solution XY Plot dialog box. Figure 9.10: wall-6 RNG k-ɛ and Standard k-ɛ Solutions (x = 0 cm to x = 43 cm) 9-32 Release 12.0 c ANSYS, Inc. March 12, 2009

Summary This tutorial illustrated the setup and solution of a 2D, axisymmetric disk cavity problem in ANSYS FLUENT. The ability to calculate a swirl velocity permits the use of a 2D mesh, thereby making the calculation simpler and more economical to run than a 3D model. This can be important for problems where the enhanced wall treatment is used, and the near-wall flow field is resolved using a fine mesh (the first mesh point away from the wall being placed at a y+ on the order of 1). For more information about mesh considerations for turbulence modeling, see Section 12.3 in the separate User s Guide. Further Improvements The case modeled in this tutorial lends itself to parametric study due to its relatively small size. Here are some things you may wish to try: Separate wall-6 into two walls. Mesh Separate Faces... Specify one wall to be stationary, and rerun the calculation. Use adaption to see if resolving the high velocity and pressure-gradient region of the flow has a significant effect on the solution. Introduce a non-zero swirl at the inlet or use a velocity profile for fully-developed pipe flow. This is probably more realistic than the constant axial velocity used here, since the flow at the inlet is typically being supplied by a pipe. Model compressible flow (using the ideal gas law for density) rather than assuming incompressible flow text. This tutorial guides you through the steps to reach an initial solution. You may be able to obtain a more accurate solution by using an appropriate higher-order discretization scheme and by adapting the mesh. Mesh adaption can also ensure that the solution is independent of the mesh. These steps are demonstrated in Tutorial 1. References 1. Pincombe, J.R., Velocity Measurements in the Mk II - Rotating Cavity Rig with a Radial Outflow, Thermo-Fluid Mechanics Research Centre, University of Sussex, Brighton, UK, 1981. Release 12.0 c ANSYS, Inc. March 12, 2009 9-33

9-34 Release 12.0 c ANSYS, Inc. March 12, 2009