Fluent - Tutorials
In this section I will be updating the tutorial and detail procedure to setup the problem in various commercial and non commercial software's. Keep checking it frequently for the updates..In this section I will be updating the tutorial and detail procedure to setup the problem in various commercial and non commercial software's. Keep checking it frequently for the updates..
Please check out the link below to find out more:
If you are looking for some specific cases to be included please leave a note in the forum section
Modeling Turbulent Flow in a Mixing
The purpose of this tutorial is to illustrate the setup and solution of a 3D turbulent ﬂuid ﬂow for periodic section of a mixing tank.
Mixing is a very crucial unit operation in process industry. The efficiency of mixing depends on the type of agitator that will provide the required level of mixing in as short time as possible. Mixing time is usually the critical parameter in determining the eﬃciency of an agitated system. A CFD analysis yields values for species concentration, ﬂuid velocity and temperature throughout the solution domain. This allows engineers to evaluate alternative designs and choose the optimum conﬁguration.
This tutorial demonstrates how to do the following:
This tutorial assumes that you have little experience with FLUENT but are familiar with the interface.
Consider a cylindrical vessel of diameter (T) 1 m, ﬁlled with water up to H = T. The ﬂuid is stirred by a standard six-blade Rushton turbine (Figure 9.1 ) rotating at a speed of 50 rpm. The turbine diameter (D) = T/3, blade height = D/5, and blade width = D/4.
Figure 9.1: Schematic of Impeller
Setup and Solution Step 1: Grid
1. Read the grid ﬁle, tank.msh.
File −→ Read −→Case...
FLUENT will read the mesh ﬁle and report the progress in the console.
2. Check the grid.
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.
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.
(a) Close the Scale Grid panel.
4. Display the grid.
(a) Click the Colors... button to open the Grid Colors panel.
i. Select Color by ID in the Options group box.
ii. Close the Grid Colors panel.
(b) Click Display in the Grid Display panel (Figure 9.2 ).
Figure 9.2: Grid Display
As the grid lines for all the zones are visible, the display looks cluttered. For clear visibility, enable the Hidden Line Removal option.
5. Display the grid without hidden lines.
(a) Enable Hidden Line Removal in the Rendering group box.
Figure 9.3: Grid Display Without Hidden Lines
(d) Close the Grid Display panel.
Step 2: Models
1. Enable the RNG k-epsilon model.
As the ﬂow is turbulent, use a suitable turbulence model. For mixing tanks, it is recommended that you use the RNG k-epsilon model to resolve the correct ﬂow features.
Deﬁne −→ Models −→Viscous...
Step 3: Materials
1. Add liquid water to the list of ﬂuid materials by copying it from the materials database.
(a) Click the Fluent Database... button to open the Fluent Database Materials panel.
i. Select water-liquid (h2o<l>) from the Fluent Fluid Materials selection list.
This will display the default settings for water-liquid.
ii. Click Copy and close the Fluent Database Materials panel.
(b) Click Change/Create and close the Materials panel.
Step 4: Units
You can change the units of variables if required. The problem speciﬁes angular velocity in rpm whereas the default unit is rad/s.
1. Change the unit of angular velocity.
Step 5: Boundary Conditions
The problem is solved using rotating reference frame for the ﬂuid. The turbine wall will then be deﬁned to rotate with the moving frame.
Deﬁne −→Boundary Conditions...
1. Set the boundary conditions for moving-zone.
i. Select water-liquid from the Material Name drop-down list.
ii. Select Moving Reference Frame from the Motion Type drop-down list.
iii. Enter 50 rpm for Speed and click OK to close the Fluid panel.
2. Set the boundary conditions for tank.
i. Select water-liquid from the Material Name drop-down list.
ii. Click OK to close the Fluid panel.
3. Set the boundary conditions for wall zones and retain the default settings for turbine wall.
For a rotating reference frame, FLUENT assumes by default that all walls adjacent to the moving-zone rotate with the speed of moving reference frame. Hence all walls will rotate with respect to stationary (absolute) reference frame.
To specify a non-rotating wall, set a rotational speed of zero in the absolute frame. As the outer-shaft is a part of non-rotating ﬂuid zone, explicitly set the rotation for this boundary.
(a) Select outer-shaft from the Zone selection list.
(b) Click the Set... button to open the Wall panel.
i. Select Moving Wall from the Wall Motion drop-down list.
ii. Select Absolute and Rotational in the Motion group box.
iii. Enter 50 rpm for Speed and click OK to close the Wall panel.
4. Set the boundary condition for periodic zones.
5. Close the Boundary Conditions panel.
Step 6: Solution
1. Retain the default solver settings.
Solve −→ Controls −→Solution...
2. Initialize the ﬂow.
Solve −→ Initialize −→Initialize...
(a) Click Init and close the Solution Initialization panel.
The ﬂow will get initialized with the default values of velocity and turbulence quantities.
3. Enable the plotting of residuals during the calculation.
Solve −→ Monitors −→Residual...
4. Save the case ﬁle (tank1.cas.gz).
File −→ Write −→Case...
Retain the default Write Binary Files option so that you can write a binary ﬁle. The .gz extension will save compressed ﬁles on both, Windows and Linux/UNIX platforms.
5. Start the calculation by requesting 1200 iterations.
(a) Set Number of Iterations to 1200.
(b) Click Iterate.
The solution converges in approximately 1170 iterations with the default convergence criteria. The residuals plot is shown in Figure 9.4
(c) Close the Iterate panel.
The default convergence criteria are not suﬃcient to get the correct ﬂow features in a mixing tank. To judge the convergence, some of the integrated quantities needs to be monitored along with velocity magnitude around the turbine.
In this problem, monitor the velocity magnitude on a surface just above and below the turbine. Also monitor the volume integral of kinetic energy in the tank.
Figure 9.4: Scaled Residuals
6. Create isosurfaces.
(a) Select Grid... and Z-Coordinate from the Surface of Constant drop-down lists.
(b) Enter 0.56 for Iso-Values.
(c) Enter z=0.56 for New Surface Name.
7. Create a custom ﬁeld function for kinetic energy, (0.5*density*velocity-magnitude*velocity-magnitude).
This custom ﬁeld function can be used like any other standard variable reported by FLUENT. The value of the quantity will be evaluated at cell centers using the cell variables used in the deﬁnition.
Deﬁne −→Custom Field Functions...
(f) Select Velocity... and Velocity Magnitude from the Field Functions drop-down lists.
(g) Click Select and click the X button again.
(h) Select Velocity... and Velocity Magnitude from the Field Functions drop-down lists.
(i) Click Select.
8. Set the surface monitors.
Solve −→ Monitors −→Surface...
9. Set the volume monitors.
Solve −→ Monitors −→Volume...
10. Disable the convergence criteria for all the equations.
For a better convergence, perform the iterations till all the monitors ﬂatten out. Therefore, disable the convergence criteria.
Solve −→ Monitors −→Residual...
Figure 9.5: Surface Monitor for Velocity Magnitude on z = 0.56
Figure 9.6: Surface Monitor for Velocity Magnitude on z = 0.64
Figure 9.7: Volume Monitor for ke
12. Save the case and data ﬁles (tank2.cas.gz and tank2.dat.gz).
File −→ Write −→Case & Data...
Step 7: Postprocessing
1. Create an angular co-ordinate.
(a) Select Grid... and Angular Coordinate from the Surface of Constant drop-down lists.
(b) Enter -120 for Iso-Values.
(c) Enter angular=-120 for New Surface Name and click Create.
(d) Close the Iso-Surface panel.
2. Display velocity vectors on an iso-surface created using angular co-ordinate (Figure 9.8 ).
(a) Select Velocity from the Vectors of drop-down list.
(b) Select Velocity... and Velocity Magnitude from the Color by drop-down lists.
i. Enable Fixed Length.
This allows you to display all the vectors with the same length.
ii. Click Apply and close the Vector Options panel.
There are two circulation loops which enhance mixing, one at the top of the turbine and another below.
Figure 9.8: Velocity Vectors on angular = -120
3. Display turbulent kinetic energy on the periodic surfaces (Figure 9.9 ).
(a) Select Turbulence... and Turbulent Kinetic Energy from the Contours of drop-down lists.
Figure 9.9: Contours of Turbulent Kinetic Energy on Periodic Surfaces
4. Change the view so that results can be viewed for complete domain.
(a) Click the Deﬁne... button in the Periodic Repeats group box to open the Graphics Periodicity panel.
i. Click the Set button.
The display in graphics window will get updated and will repeat the surfaces six times.
ii. Close the Graphics Periodicity panel.
(b) Click Apply and close the Views panel.
5. Display the velocity contours on surface, turbine (Figure 9.10 ).
(a) Select Velocity... and Velocity Magnitude from the Contours of drop-down lists.
Figure 9.10: Contours of Velocity Magnitude on turbine
This example demonstrates the use of moving reference frame (MRF) to model the ﬂow in mixing tanks. Monitors were used to judge convergence of crucial quantities. In actual CFD analysis, much ﬁner mesh needs to be employed around the blade to resolve the velocity and pressure gradients correctly.
M. Campolo, F. Sbrizzai, A. Soldati, Time-dependent ﬂow structure and Lagrangian mixing in Ruston-impeller baﬄed-tank reactor, Chemical Engineering Science 58 (2003) 1615-1629.