Non-Newtonian Transitional Flow in an Eccentric Annulus

Size: px

Start display at page:

Download "Non-Newtonian Transitional Flow in an Eccentric Annulus"

Leslie Copeland
5 years ago
Views:

1 Tutorial 8. Non-Newtonian Transitional Flow in an Eccentric Annulus Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D, turbulent flow of a non-newtonian fluid. Turbulent non-newtonian flows are often encountered in the oil and gas industry. These fluids are used in the drilling of oil wells to transport the cuttings to the surface, and to keep solids in suspension during stationary periods. In directional drilling, where an eccentric annulus is often used, there is a tendency for the cuttings to accumulate in the narrowest gap where the velocity is lowest. Since turbulence tends to suppress such accumulation, knowledge of the velocity profiles in the annulus are essential in the design and operation of these drills. In this tutorial, you will learn how to: Read an existing mesh file in FLUENT. Check the grid for dimensions and quality. Set up the material for non-newtonian viscosity and switch to turbulence formulation for the same using text user interface (TUI) commands. Solve a time dependent simulation. Set up periodic flow conditions in FLUENT. Set up transitional flow conditions using k ω turbulence model. Create isosurfaces and isoclips for postprocessing. Examine the results and compare them with experimental data. Prerequisites This tutorial assumes that you have little experience with FLUENT but are familiar with the interface. c Fluent Inc. August 18,

Problem Description A periodic section of the eccentric annulus arrangement is considered (Figure 8.1). The inner and outer cylinders diameters are 20 mm and 40.3 mm respectively.

2 Problem Description A periodic section of the eccentric annulus arrangement is considered (Figure 8.1). The inner and outer cylinders diameters are 20 mm and 40.3 mm respectively. The inner cylinder is rotating with speed of 300 rpm whereas the outer one is stationary. The viscosity is governed by the Power law as: µ = K γ (n 1) where, n = power law index = 0.75 K = consistency index = γ = local shear rate The flow is considered to be in transitional regime with Re = Figure 8.1: Problem Schematic 8-2 c Fluent Inc. August 18, 2005

3 Preparation 1. Copy the following files to your working directory: annulus.msh non-dimensional.scm axial-p1.xy axial-p2.xy axial-p3.xy tangential-p1.xy tangential-p2.xy tangential-p3.xy 2. Start the 3D double precision solver of FLUENT. Setup and Solution Step 1: Grid 1. Read the mesh file, annulus.msh. File Read Case... FLUENT will read the mesh file and report the progress in the console window. 2. Check the grid. Grid Check This procedure checks the integrity of the mesh. Make sure the reported minimum volume is a positive number. 3. Check the scale of the grid. Grid Scale... Check the domain extents to see if they correspond to the actual physical dimensions. If not, the grid has to be scaled with proper units. In this case, the outer diameter should be 40.3 mm, therefore scale the grid in mm. c Fluent Inc. August 18,

4 (a) Select mm in the Grid Was Created In drop-down list. (b) Click Scale and close the panel. 4. Display the grid (Figures 8.2). Display Grid... The color for each periodic boundary is Cyan and for each wall it is White. FLUENT will automatically color each boundary based on its type. 8-4 c Fluent Inc. August 18, 2005

is made finer compared to the central region.

5 5. Remove the Hidden lines. Display Options... (a) Enable Hidden Line Removal and click Apply. Figure 8.2: Grid Display To capture the sharp gradients near the walls correctly, the grid adjacent to the walls is made finer compared to the central region. In addition, as the problem is turbulent it is essential to meet the correct Y+ conditions as per the wall treatment to be used. c Fluent Inc. August 18,

Step 2: Models The flow has Reynolds number of 9000, and it needs to be modeled as turbulent. The k ω model can be used for such low Reynolds number, turbulent, or transitional flows.

6 Step 2: Models The flow has Reynolds number of 9000, and it needs to be modeled as turbulent. The k ω model can be used for such low Reynolds number, turbulent, or transitional flows. R e = ρ U b d h µ (8.1) In this case, the mass flow rate = kg/s. Therefore, the bulk velocity can be calculated as: Bulkvelocity = Massflow = Density Area Where, ρ = density of the fluid = 1000 kg/m3 U b = bulk velocity = 2.72 m/s d h = hydraulic diameter (Do-Din) = µ = viscosity at the wall = (measured experimentally [1]) 1. Enable viscous model. Define Models Viscous... (a) Under Model, select k-omega (2 eqn). (b) Under k-omega Options, enable Transitional Flows. (c) Click OK. 8-6 c Fluent Inc. August 18, 2005

To enable the model, issue the text user interface command as:

7 Step 3: Materials 1. Change the material properties. Define Materials... (a) There is no model that can be used for viscosity as we need non-newtonian power law. To enable the model, issue the text user interface command as: define/models/viscous/turbulence-expert/turb-non-newtonian Enable turbulence for non-newtonian fluids? [no] yes c Fluent Inc. August 18,

(b) In the materials panel, select non-newtonian-power-law in the Viscosity dropdown list. This opens Non-Newtonian Power Law panel. i. Specify the following parameters: ii.

0001 Maximum Viscosity Limit 1000 (d) Specify Name as cmc and click Change/Create. (e) Click NO when FLUENT asks Change/Create mixture and overwrite air?

8 (b) In the materials panel, select non-newtonian-power-law in the Viscosity dropdown list. This opens Non-Newtonian Power Law panel. i. Specify the following parameters: ii. Click OK. (c) Set Density to Parameter Value Consistency Index Power-Law Index 0.75 Reference Temperature 0 Minimum Viscosity Limit Maximum Viscosity Limit 1000 (d) Specify Name as cmc and click Change/Create. (e) Click NO when FLUENT asks Change/Create mixture and overwrite air? (f) Close the materials panel. FLUENT automatically enables the energy equation as non-newtonian power law formulation is being used. You can disable it from the solution afterwards. 8-8 c Fluent Inc. August 18, 2005

Step 5: Boundary Conditions 1. Set the boundary conditions for fluid. Define Boundary Conditions.

9 Step 4: Units 1. Change the units for angular-velocity to rpm. Define Units... (a) Under Quantities, select angular-velocity. (b) Under Units, select rpm and close the panel. Step 5: Boundary Conditions 1. Set the boundary conditions for fluid. Define Boundary Conditions... (a) Under Zone, select fluid. The Type will be reported as fluid. (b) Click Set... The Fluid panel opens. c Fluent Inc. August 18,

Set the boundary conditions for inner. (a) Under Zone, select inner.

10 i. Select cmc in the Material Name drop-down list. ii. Click OK to accept the settings and close the panel. 2. Set the boundary conditions for inner. (a) Under Zone, select inner. The Type will be reported as wall. (b) Click Set... The Wall panel opens c Fluent Inc. August 18, 2005

Click OK. Step 6: Periodic Conditions 1.

11 i. Select Momentum tab. ii. Under Wall Motion, enable Moving Wall. iii. Under Motion, enable Rotational and specify a value of 300 for Speed. iv. Click OK. Step 6: Periodic Conditions 1. Specify the flow rate across periodic boundaries. Define Periodic Conditions... c Fluent Inc. August 18,

12 (a) Under Type, enable Specify Mass Flow. (b) Under Flow Direction, set the values of X, Y, and Z to 0, 0, and 1 respectively. (c) Specify a value of for Mass Flow Rate. (d) Click OK to accept the settings and close the panel. Step 7: Solution 1. Set the solution controls. Solve Controls Solution... (a) Under Equations, deselect Energy. The viscosity is function of shear stress (does not depend on the temperature). Therefore, there is no need to solve the energy equation. (b) Retain other settings and click OK. 2. Initialize the flow. Solve Initialize Initialize c Fluent Inc. August 18, 2005

(a) Set Z Velocity (m/s) to 2.72. From Equation 8.1, bulk velocity was calculated as 2.72. (b) Set Turbulence Kinetic Energy to 0.

Enable plotting of residuals during the calculation. Solve Monitors Residuals... (a) Under Options, enable Plot.

13 (a) Set Z Velocity (m/s) to From Equation 8.1, bulk velocity was calculated as (b) Set Turbulence Kinetic Energy to (c) Set Specific Dissipation Rate to (d) Click Init and close the panel. 3. Enable plotting of residuals during the calculation. Solve Monitors Residuals... (a) Under Options, enable Plot. (b) Click OK. 4. Save the case file (annulus1.cas.gz). File Write Case... c Fluent Inc. August 18,

Retain the default activated Write Binary Files option so that you can write a binary file. The.gz option will save zipped files, this will work on both, Windows as well as UNIX platforms. 5.

14 Retain the default activated Write Binary Files option so that you can write a binary file. The.gz option will save zipped files, this will work on both, Windows as well as UNIX platforms. 5. Iterate the solution. Solve Iterate... (a) Set Number of Iterations to 400. (b) Click Iterate to start the calculation. The solution converges in 283 iterations. The residuals plot is shown in Figure c Fluent Inc. August 18, 2005

15 Figure 8.3: Scaled Residuals 6. Switch to higher order upwind schemes. Solve Controls Solution... (a) Under Discretization, select QUICK for Momentum, Turbulence Kinetic Energy, and Specific Dissipation Rate. (b) Click OK. Convergence can be detected by monitoring some key parameter during the iterations. In this case you will monitor turbulence kinetic energy over central plane of the domain. To do so, create an isosurface at the corresponding location in the domain. c Fluent Inc. August 18,

Monitor the turbulence kinetic energy over the isosurface. Solve Monitor Surface... (a) Increase Surface Monitors to 1.

16 7. Create an isosurface. Surface Iso-Surface... (a) Under Surface of Constant, select Grid... and Y-Coordinate. (b) Under Iso-Values, enter 0. (c) Under New Surface Name, enter y=0. (d) Click Create and close the panel. 8. Monitor the turbulence kinetic energy over the isosurface. Solve Monitor Surface... (a) Increase Surface Monitors to 1. (b) Enable Plot and Print for monitor-1. (c) Click Define... This opens Define Surface Monitor panel c Fluent Inc. August 18, 2005

i. Select Area Weighted Average in the Report Type drop-down list. ii. Select Turbulence... and Turbulence Kinetic Energy in the Reports of dropdown lists. iii. Under Surface, select y=0. iv.

17 i. Select Area Weighted Average in the Report Type drop-down list. ii. Select Turbulence... and Turbulence Kinetic Energy in the Reports of dropdown lists. iii. Under Surface, select y=0. iv. Click OK. (d) Click OK in the Surface Monitors panel. The average value of turbulence kinetic energy on y=0 plane will be plotted in the graphics window and printed on the console during the iterations. 9. Disable convergence criteria for all equations. Solve Monitors Residuals... (a) Disable Check Convergence for all equations. (b) Click OK. c Fluent Inc. August 18,

18 10. Iterate the solution till the convergence is achieved. Solve Iterate... (a) Set Number of Iterations to (b) Click Iterate to start the calculation. The solution will converge in around 4500 iterations. It is observed that the monitor plot is almost flat and you can stop the computation. Figure 8.4: Convergence History of Turbulence Kinetic Energy on y=0 Figure 8.5: Scaled Residuals 11. Save the case and data files (annulus2.cas.gz and annulus2.dat.gz). File Write Case & Data c Fluent Inc. August 18, 2005

19 Step 8: Postprocessing 1. Create an isosurface. The flow is translationally periodic along Z direction. Create an isosurface along Z direction to view the results. Surface Iso-surface... (a) Select Grid... and Z-Coordinate in the Surface of Constant drop-down lists. (b) Click Compute. Min and Max values will get updated as per the domain extents. (c) Under Iso-Values, enter (d) Enter New Surface Name as z= (e) Click Create and close the panel. 2. Display velocity vectors (Figure 8.6). Display Vectors... c Fluent Inc. August 18,

005. (d) Click Display and close the panel. Figure 8.6: Velocity Vectors on z=0.005 3.

20 (a) Select Velocity, in the Vectors of drop-down list. (b) Select Velocity... and Velocity Magnitude in the Color by drop-down lists. (c) Under Surfaces, select z= (d) Click Display and close the panel. Figure 8.6: Velocity Vectors on z= Display filled contours of molecular viscosity (Figure 8.7). Display Contours c Fluent Inc. August 18, 2005

Observe the shear thinning behavior of the fluid.

21 (a) Select Properties... and Molecular Viscosity in the Contours of drop-down lists. (b) Under Options, enable Filled. (c) Under Surfaces, select z= (d) Click Display and close the panel. Observe the shear thinning behavior of the fluid. The viscosity is less near walls (high shear regions) and it is high in the central part (low shear regions). Figure 8.7: Contours of Molecular Viscosity on z=0.005 c Fluent Inc. August 18,

22 4. Calculate the pressure drop. Define Periodic Conditions... It is important to know the pressure drop in any flow system. FLUENT updates the pressure gradient value after every iteration in the Periodic Conditions panel. Multiply the value reported of pressure gradient by the length of periodic section to get the pressure drop value. In literature, the results are available at three lines P1, P2 and P3 as shown in Figure 8.1. We can create them on the z= surface. 5. Create another isosurface to view the results. Surface Iso-surface... (a) Under From Surface, select z= (b) Select Grid... and Y-Coordinate, in the Surface of Constant drop-down lists. (c) Under Iso-Values, retain the value of 0. (d) Enter New Surface Name as plane. (e) Click Create and close the panel c Fluent Inc. August 18, 2005

(d) Specify 0 for Min. (e) Change New Surface Name to p-1 and click Clip. A new surface (p-1) will be added to the list of surfaces.

23 6. Create isoclips. Surface Iso-Clip... (a) Under Clip Surface list, select plane. (b) Select Grid... and X-Coordinate in the Clip to Values drop-down lists. (c) Click Compute. This will display Min and Max values of x-coordinate along plane. (d) Specify 0 for Min. (e) Change New Surface Name to p-1 and click Clip. A new surface (p-1) will be added to the list of surfaces. (f) Click Compute. (g) Similarly, clip plane surface with a value of 0 for Max field of X-coordinate and name it as p Create a line. Surface Line/Rake... c Fluent Inc. August 18,

(a) Retain the default values of x0 and x1. The x0 and x1 values correspond to the X center of the domain (b) Specify a value of 0 for y0 and any number greater than 0.02015 (say 0.

24 (a) Retain the default values of x0 and x1. The x0 and x1 values correspond to the X center of the domain (b) Specify a value of 0 for y0 and any number greater than (say 0.1, in this case) for y1. (c) Set z0 and z1 to This will place the line in the central plane. (d) Enter p-2 as New Surface Name. (e) Click Create and close the panel. 8. Display all three surfaces that you have created (Figure 8.8). Display Grid... (a) Under Surfaces, select p-1, p-2, p-3 and z= (b) Under Edge Type, select Outline. (c) Click Display to verify the correct positions of these planes c Fluent Inc. August 18, 2005

Figure 8.8: Grid Display of New Surfaces 9. Read the scheme file. To non-dimensionalize the plots along three planes p-1, p-2, and p-3, read in the scheme file provided with this tutorial.

25 Figure 8.8: Grid Display of New Surfaces 9. Read the scheme file. To non-dimensionalize the plots along three planes p-1, p-2, and p-3, read in the scheme file provided with this tutorial. This file has the pre-defined custom field functions based on the correct values. Reading this file will make many custom field functions available for postprocessing. File Read Scheme... (a) Select non-dimensional.scm and click OK. c Fluent Inc. August 18,

Read the xy files, provided with this tutorial, that contains the experimental data. Plot XY Plot... (a) Click Load File.

26 10. View the definitions of custom field functions. Define Custom Field Functions... (a) View the definition of each custom field function by clicking Manage Read the xy files, provided with this tutorial, that contains the experimental data. Plot XY Plot... (a) Click Load File... This opens a Select File dialog box. i. Select axial-p1.xy, axial-p2.xy, axial-p3.xy, tangential-p1.xy, tangential-p2.xy, and tangential-p3.xy and click OK. This will make axial and tangential velocities available in normalized form for comparison c Fluent Inc. August 18, 2005

(b) Compare the normalized axial velocity along p1 (Figure 8.9). i. Under Options, disable Node Values and Position on X axis. ii. Select Custom Field Functions.

27 (b) Compare the normalized axial velocity along p1 (Figure 8.9). i. Under Options, disable Node Values and Position on X axis. ii. Select Custom Field Functions... and normalized-axial in the Y Axis Function drop-down lists. iii. Select Custom Field Functions... and normalized-p1 in the X Axis Function drop-down lists. iv. Under Surfaces, select p1. v. Under File Data, select normalized-axial vs. normalized-p1 and click Plot. Figure 8.9: FLUENT Results vs Experimental Data for Axial Velocity Component at p-1 c Fluent Inc. August 18,

28 (c) Compare normalized tangential velocity along p3 (Figure 8.10). i. Under Options, disable Position on X axis. ii. Select Custom Field Functions... and normalized-tangential in the Y Axis Function drop-down lists. iii. Select Custom Field Functions... and normalized-p3 in the X Axis Function drop-down lists. iv. Under Surfaces, select p3. v. Under File Data, select normalized-tangential vs normalized-p3 and click Plot. Figure 8.10: FLUENT Results vs Experimental Data for Tangential Velocity Component at p c Fluent Inc. August 18, 2005

29 (d) Similarly, compare remaining results as shown in Figures 8.11 and Figure 8.11: FLUENT Results vs Experimental Data for Axial Velocity Component at p-2 and p3 Figure 8.12: FLUENT Results vs Experimental Data for Tangential Velocity Component at p-1 and p2 c Fluent Inc. August 18,

30 Summary This tutorial demonstrated a similarity between the axial and tangential velocity profiles predicted by FLUENT and the experimental data. You also studied, the performance of k ω model in transitional regime along with the non-newtonian formulation of viscosity. The use of monitors for detecting convergence is highlighted. References 1. J. M. Nouri and J. H. Whitelaw, Flow of Newtonian and non-newtonian fluids in an eccentric annulus with rotation of inner cylinder, International Journal of Heat and Fluid Flow 18: , 1997 Exercises/ Discussions 1. How will the results vary if: (a) The direction of rotation of inner cylinder is reversed. (b) The inner cylinder rotates with higher RPM. (c) The outer cylinder is made to rotate in the same direction as that of inner cylinder. (d) The flow is simulated as inviscid. 2. Will the same grid work if the mass flow across the periodic boundaries is increased 10 times from the existing value? What changes would you suggest in the case set-up? 3. What other situation can be simulated using the same mesh file. Links for Further Reading c Fluent Inc. August 18, 2005

Simulation of Flow Development in a Pipe

Tutorial 4. Simulation of Flow Development in a Pipe Introduction The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent fluid flow in a pipe. The pipe networks are common