PDF
Swirl Flow Around a Rotating Disk
Introduction
This example models a rotating disk in a tank. The model geometry is shown in Figure 1. Because the geometry is rotationally symmetric, it is possible to model it as a 2D cross section. However, the velocities in the angular direction differ from zero, so the model must include all three velocity components, even though the geometry is in 2D.
Figure 1: The original 3D geometry can be reduced to 2D because the geometry is rotationally symmetric.
Model Definition
Domain Equations
The flow is described by the Navier-Stokes equations:
In these equations, u denotes the velocity (SI unit: m/s), ρ the density (SI unit: kg/m3), μ the dynamic viscosity (SI unit: Pa·s), and p the pressure (SI unit: Pa). For a stationary, axisymmetric flow the equations reduce to (Ref. 1):
Here u is the radial velocity, v the rotational velocity, and w the axial velocity (SI unit: m/s). In the model you set the volumetric force components Fr, , and Fz to zero. The swirling flow is 2D even though the model includes all three velocity components.
Boundary Conditions
Figure 2 below shows the boundary conditions.
Figure 2: Boundary conditions.
On the stirrer, use the sliding wall boundary condition to specify the velocities. The velocity components in the plane are zero, and that in the angular direction is equal to the angular velocity, ω, times the radius, r:
At the boundaries representing the cylinder surface a no slip condition applies, stating that all velocity components equal zero:
At the boundary corresponding to the rotation axis, use the axial symmetry boundary condition allowing flow in the tangential direction of the boundary but not in the normal direction. This is obtained by setting the radial velocity to zero:
On the top boundary, which is a free surface, use the Symmetry condition to allow for flow in the axial and rotational directions only. The boundary condition is mathematically similar to the axial symmetry condition.
Point Settings
In this model you need to lock the pressure to a reference value in a point. The reason for this is that the model does not contain any boundary condition where the pressure is specified (this is often done at outlets). Also the fluid density is constant, which means that the pressure level is not coupled to the density. In this model, set the pressure to zero in the top-right corner.
Results
The parametric solver provides the solution for four different angular velocities. Figure 3 shows the results for the smallest angular velocity, ω = 0.25π rad/s.
Figure 3: Results for angular velocity ω= 0.25π rad/s. The surface plot shows the magnitude of the velocity field and the white lines are streamlines of the velocity field.
The shape of the two recirculation zones, which are visualized with streamlines, changes as the angular velocity increases. Figure 4 shows the streamlines of the velocity field for higher angular velocities.
Figure 4: Results for angular velocities ω =  0.5π, 2π, and 4π rad/s. The surface plot shows the magnitude of the velocity and the white lines are streamlines of the velocity field.
Figure 5 and Figure 6 show isocontours of the rotational velocity component together with surface plots of the velocity magnitude for different angular velocities.
.
Figure 5: Isocontours for the azimuthal velocity component for angular velocity ω = 0.25π rad/s. The surface plot shows the magnitude of the velocity.
Figure 6: Magnitude of the velocity field (surface) and isocontours for the azimuthal velocity component for angular velocities (left to right) ω = 0.5π, 2π, and 4π rad/s.
Figure 7 shows the turbulent viscosity and flow fields for the angular velocity to ω = 500π rad/s and turbulent flow in the mixer volume.
Figure 7: Results for angular velocity ω = 500π rad/s. The surface plot shows the turbulent viscosity and the white lines are streamlines of the velocity field.
Reference
1. P.M. Gresho and R.L. Sani, Incompressible Flow and the Finite Element Method, vol. 2, p. 469, John Wiley & Sons, 1998.
Application Library path: CFD_Module/Single-Phase_Flow/rotating_disk
Modeling Instructions
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  2D Axisymmetric.
2
In the Select Physics tree, select Fluid Flow>Single-Phase Flow>Laminar Flow (spf).
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
omega
0.25*pi[rad/s]
0.7854 rad/s
Angular velocity
Geometry 1
Rectangle 1 (r1)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 0.02.
4
In the Height text field, type 0.04.
5
Click  Build All Objects.
6
Click the  Zoom Extents button in the Graphics toolbar.
Rectangle 2 (r2)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 0.008.
4
In the Height text field, type 0.003.
5
Locate the Position section. In the z text field, type 0.014.
6
Click  Build All Objects.
Rectangle 3 (r3)
1
In the Geometry toolbar, click  Rectangle.
2
In the Settings window for Rectangle, locate the Size and Shape section.
3
In the Width text field, type 0.001.
4
In the Height text field, type 0.023.
5
Locate the Position section. In the z text field, type 0.017.
6
Click  Build All Objects.
Difference 1 (dif1)
1
In the Geometry toolbar, click  Booleans and Partitions and choose Difference.
2
Select the object r1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the  Activate Selection toggle button.
5
Select the objects r2 and r3 only.
6
Clear the Keep interior boundaries check box.
7
Click  Build All Objects.
8
Click the  Zoom Extents button in the Graphics toolbar.
Materials
Material 1 (mat1)
1
In the Model Builder window, under Component 1 (comp1) right-click Materials and choose Blank Material.
2
In the Settings window for Material, locate the Material Contents section.
3
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Density
rho
1e3
kg/m³
Basic
Dynamic viscosity
mu
1e-3
Pa·s
Basic
Laminar Flow (spf)
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
In the Settings window for Laminar Flow, locate the Physical Model section.
3
Select the Swirl flow check box.
4
Click to expand the Discretization section. From the Discretization of fluids list, choose P2+P1.
This setting gives quadratic elements for the velocity field.
Wall 2
1
In the Physics toolbar, click  Boundaries and choose Wall.
2
Select Boundaries 3–5 and 7 only.
3
In the Settings window for Wall, click to expand the Wall Movement section.
4
Select the Sliding wall check box.
5
In the vw text field, type omega*r.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundary 6 only.
Pressure Point Constraint 1
1
In the Physics toolbar, click  Points and choose Pressure Point Constraint.
2
Select Point 8 only.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, click to expand the Study Extensions section.
3
Select the Auxiliary sweep check box.
4
Click  Add.
5
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
omega (Angular velocity)
0.25*pi 0.5*pi 2*pi 4*pi
rad/s
6
In the Home toolbar, click  Compute.
Results
Velocity (spf)
To create Figure 3 do the following steps:
1
In the Settings window for 2D Plot Group, locate the Data section.
2
From the Parameter value (omega (rad/s)) list, choose 0.7854.
3
In the Velocity (spf) toolbar, click  Plot.
Surface
1
In the Model Builder window, expand the Velocity (spf) node, then click Surface.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose mm/s.
Streamline 1
1
In the Model Builder window, right-click Velocity (spf) and choose Streamline.
2
In the Settings window for Streamline, locate the Streamline Positioning section.
3
From the Positioning list, choose Uniform density.
4
Locate the Coloring and Style section. Find the Point style subsection. From the Type list, choose Arrow.
5
Select the Number of arrows check box.
6
In the associated text field, type 100.
7
From the Color list, choose Gray.
8
Locate the Streamline Positioning section. In the Separating distance text field, type 0.04.
9
In the Velocity (spf) toolbar, click  Plot.
To produce the series of snapshots of the velocity and streamlines of the velocity field shown in Figure 4, proceed with the following steps:
Surface
1
In the Model Builder window, click Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
Clear the Color legend check box.
Velocity (spf)
1
In the Model Builder window, click Velocity (spf).
2
In the Settings window for 2D Plot Group, locate the Data section.
3
From the Parameter value (omega (rad/s)) list, choose 1.5708.
4
In the Velocity (spf) toolbar, click  Plot.
5
From the Parameter value (omega (rad/s)) list, choose 6.2832.
6
In the Velocity (spf) toolbar, click  Plot.
7
From the Parameter value (omega (rad/s)) list, choose 12.566.
8
In the Velocity (spf) toolbar, click  Plot.
To plot the isocontours for the azimuthal velocity component Figure 5, proceed with the following steps.
Azimuthal Velocity
1
In the Home toolbar, click  Add Plot Group and choose 2D Plot Group.
2
In the Settings window for 2D Plot Group, type Azimuthal Velocity in the Label text field.
3
Locate the Data section. From the Parameter value (omega (rad/s)) list, choose 0.7854.
Surface 1
Right-click Azimuthal Velocity and choose Surface.
Contour 1
1
In the Model Builder window, right-click Azimuthal Velocity and choose Contour.
2
In the Settings window for Contour, click to expand the Quality section.
3
In the Azimuthal Velocity toolbar, click  Plot.
4
Click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Laminar Flow>Velocity and pressure>Velocity field - m/s>v - Velocity field, phi component.
5
Locate the Levels section. In the Total levels text field, type 15.
6
Locate the Coloring and Style section. From the Coloring list, choose Uniform.
7
From the Color list, choose Gray.
8
Locate the Quality section. From the Resolution list, choose Finer.
9
From the Recover list, choose Within domains.
To reproduce Figure 6 do the following steps.
Surface 1
1
In the Model Builder window, click Surface 1.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
Clear the Color legend check box.
Azimuthal Velocity
1
In the Model Builder window, click Azimuthal Velocity.
2
In the Settings window for 2D Plot Group, locate the Data section.
3
From the Parameter value (omega (rad/s)) list, choose 1.5708.
4
In the Azimuthal Velocity toolbar, click  Plot.
5
From the Parameter value (omega (rad/s)) list, choose 6.2832.
6
In the Azimuthal Velocity toolbar, click  Plot.
7
From the Parameter value (omega (rad/s)) list, choose 12.566.
8
In the Azimuthal Velocity toolbar, click  Plot.
Before solving for turbulent flow, store the laminar flow solutions in a separate dataset.
9
In the Study toolbar, click  Create Solution Copy.
Study 1
Laminar Swirl Flow
1
In the Model Builder window, expand the Study 1>Solver Configurations node, then click Solution 1 - Copy 1 (sol2).
2
In the Settings window for Solution, type Laminar Swirl Flow in the Label text field.
Laminar Flow (spf)
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
In the Settings window for Laminar Flow, locate the Turbulence section.
3
From the Turbulence model type list, choose RANS.
Higher order elements are often not cost effective for turbulent flows and can also cause numerical instabilities.
4
Locate the Discretization section. From the Discretization of fluids list, choose P1+P1.
Mesh 1
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Fine.
Study 1
Step 1: Stationary
1
In the Model Builder window, under Study 1 click Step 1: Stationary.
2
In the Settings window for Stationary, locate the Study Extensions section.
3
In the table, enter the following settings:
Parameter name
Parameter value list
Parameter unit
omega (Angular velocity)
range(pi*100,pi*200,pi*500)
rad/s
The continuation solver works best for models with linear dependence on the parameter. A more robust alternative for nonlinear applications is to start from the solution for the previous parameter value.
1
From the Run continuation for list, choose No parameter.
2
From the Reuse solution from previous step list, choose Yes.
3
In the Study toolbar, click  Compute.
Results
Velocity (spf)
Now create two cut plane datasets in order visualize the velocity on the revolved solution.
Cut Plane 1
1
In the Results toolbar, click  Cut Plane.
2
In the Settings window for Cut Plane, locate the Plane Data section.
3
From the Plane type list, choose General.
4
In row Point 2, set x to 0.
5
In row Point 2, set z to 1.
6
In row Point 3, set x to cos(-90[deg]).
7
In row Point 3, set y to sin(-90[deg]).
8
Click  Plot.
Cut Plane 2
1
Right-click Cut Plane 1 and choose Duplicate.
2
In the Settings window for Cut Plane, locate the Plane Data section.
3
In row Point 3, set x to cos(135[deg]).
4
In row Point 3, set y to sin(135[deg]).
5
Click  Plot.
Surface
1
In the Model Builder window, expand the Results>Velocity, 3D (spf) node, then click Surface.
2
In the Settings window for Surface, locate the Coloring and Style section.
3
From the Color table list, choose GrayScale.
4
Clear the Color legend check box.
5
Select the Reverse color table check box.
Velocity, 3D (spf)
In the Model Builder window, click Velocity, 3D (spf).
Streamline Surface 1
1
In the Velocity, 3D (spf) toolbar, click  More Plots and choose Streamline Surface.
2
In the Settings window for Streamline Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 1.
4
From the Parameter value (omega (rad/s)) list, choose 314.16.
5
Locate the Streamline Positioning section. From the Positioning list, choose Uniform density.
6
Locate the Coloring and Style section. Find the Line style subsection. From the Type list, choose Tube.
7
Select the Radius scale factor check box.
8
In the associated text field, type 1e-4.
9
Find the Point style subsection. From the Type list, choose Arrow.
10
Select the Number of arrows check box.
11
In the associated text field, type 100.
12
Select the Scale factor check box.
13
In the associated text field, type 0.018.
Color Expression 1
1
In the Velocity, 3D (spf) toolbar, click  Color Expression.
2
In the Settings window for Color Expression, locate the Coloring and Style section.
3
From the Color table list, choose JupiterAuroraBorealis.
Streamline Surface 1
Use a Filter feature to restrict the plot to the cut plane. Note that rev1y is the y)-axis of the revolution dataset.
Filter 1
1
In the Model Builder window, right-click Streamline Surface 1 and choose Filter.
2
In the Settings window for Filter, locate the Element Selection section.
3
In the Logical expression for inclusion text field, type rev1y<0[m].
4
In the Velocity, 3D (spf) toolbar, click  Plot.
Velocity, 3D (spf)
In the Model Builder window, click Velocity, 3D (spf).
Arrow Surface 1
1
In the Velocity, 3D (spf) toolbar, click  Arrow Surface.
2
In the Settings window for Arrow Surface, locate the Data section.
3
From the Dataset list, choose Cut Plane 2.
4
From the Parameter value (omega (rad/s)) list, choose 314.16.
5
Locate the Coloring and Style section. Select the Scale factor check box.
6
In the associated text field, type 0.02.
7
Locate the Arrow Positioning section. In the Number of arrows text field, type 300.
8
Click to expand the Inherit Style section. From the Plot list, choose Streamline Surface 1.
Color Expression 1
In the Velocity, 3D (spf) toolbar, click  Color Expression.
Filter 1
1
In the Model Builder window, right-click Arrow Surface 1 and choose Filter.
2
In the Settings window for Filter, locate the Element Selection section.
3
In the Logical expression for inclusion text field, type rev1y>0[m].
Velocity (spf)
Next, define a surface plot visualizing the turbulent viscosity and the streamlines of the velocity field (Figure 7).
Turbulent viscosity
1
In the Model Builder window, right-click Velocity (spf) and choose Duplicate.
2
In the Settings window for 2D Plot Group, type Turbulent viscosity in the Label text field.
Surface
1
In the Model Builder window, expand the Turbulent viscosity node, then click Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1)>Turbulent Flow, k-ε>Turbulence variables>spf.muT - Turbulent dynamic viscosity - Pa·s.
3
Locate the Coloring and Style section. Select the Color legend check box.
4
From the Color table list, choose JupiterAuroraBorealis.