TUTORIAL:
TUTORIAL: PERFORMING FLUENT SIMULATIONS IN A STIRRING VESSELSMIXING VESSEL
Report
By
Pavlos Vlachos, Vasileios N. Vlachakis and Demetri Telionis
May 5th, 2006
Blacksburg, Virginia
Introduction
This tutorial illustrates the step- by- step setup and solution of the three -dimensional turbulent flow in agitated vessels. The Mixing Tank configuration is encountered in many industries such as in chemical, mining, pharmaceutical and biotechnological. Therefore, accurate prediction of the flow field and the turbulent characteristics (Turbulent Kinetic Energy, Dissipation Rate, Reynolds Stresses, and Vorticity) in the whole tank and especially in the vicinity of the discharge impeller region are of great importance. The reason is the presence of tThe complex phenomena that take place in a tankand have directly infulence cause in the production quality and the maintenance cost.
This tutorial is prepared after the authors conducted numerical simulations for a tank with the specific parameters of a Dorr Olive flotation system. The commercial code Fluent was used. The aim here is to provide guidance to Dorr Oliver engineers on how to use the software in order to explore the effect of different values of the parameters the shape and size of the tank and its impeller/stator system, the input power, speed, material properties and others.
More specifically, tThis tutorial will guide you how to:
ü Export the right format from a CAD program
ü Read the CAD file in Gambit
ü Make changes in the geometry (add, split, subtract faces and volumes) before undertaking in order to get prepared for the meshing process
ü Mesh the geometry, i.e. create a computational grid
ü Set the boundary cConditions for the solid and fluid
ü Import the mesh in FLUENT
ü Set the physical problem in FLUENT
ü Specify different the framess of reference : Multi Reference Frame (MRF)
ü Perform the calculation using turbulent modeling
ü Judge Convergence
ü Display the Graphics
ü Export data for importing them to a Graphics program like Tecplot or other format for further post processing.
Problem Description
The two mixing tank configurations are considered in this study. The first one is a baffled cylindrical vessel with diameter (Figure 2a). Four equally spaced baffles with widthand thickness were mounted on the tank wall. The tank was agitated by a Rushton turbine (disk with six perpendicular blades) with diameter, disk diameter, blade width, blade height blade thickness. (Figure 2b, 2c) The working fluid was water and its height was equal to the height of the tank. This model is identical to the model employed in the experimental work carried out by the present team. The second one is a conical tank agitated by a six curved blade impeller. A stator mounted in the bottom of the tank house the impeller. The whole design is patent of the Dorr-Oliver company. (Figure 3). In both sets of calculations, the origin of the coordinate system was fixed in the center of the impeller. The Reynolds number was based on the impeller diameter, Re=NDI2/ν.
Figure 1. 3D representation of the Tank agitated by the Rushton from Inventor 10
a. /
b.
c.
Figure 2. 2D representation of the Tank agitated by the Rushton impeller
a. b.
c.
Figure 3. 3D representation of the Stator, Impeller and Tank of the Dorr-Oliver configuration
In the CAD drawing in addition to the real geometry we have to add a cylindrical zone around the impeller to account for the rotational zone which is needed for both the MRF and the SG. After finalizing the geometry in a CAD program (In this study Inventor 10 was used) we save the file as a family of the IGES format which includes the following files: .igs, .ige, .iges. Then we open GAMBIT. A start up menu will come up with the following format:
Working Directory: …………………… (Browse)
Session Id: new session
Options: -r.2.2.30
We continue and automatically Exceed will run on the background as well as a new window of GAMBIT will be appeared.
1. Import the mesh
FileàImportàIGES….
Under the Filename we will browse to find our file (from now on we will refer to it
as test with the appropriate ending every time).
Import Options:
Translator: Native Spatial (Choose Spatial)
Import Sources: (Generic, AutoCAD, SolidWorks, Jama)
(Choose Generic if the 3D geometry has been made with other programs than the
three listed above)
Make Tolerant (Choose this)
Heal Geometry (Choose this option if you have stand alone vertices or faces)
2. Make changes to the geometry (add, subtract, and split volumes)
In this section we will make some changes in the geometry in order to make the meshing more convenient. not to have problems with the meshing technique. First, of all we need to know how many volumes we have and what do they represent. Let’ us take for example the Dorr-Oliver configuration, without adding the stator at this first step of this study. We propose to define the Therefore we are going to have the following five vVolumes.
A representative snapshot from the Gambit’s environment is presented in Figure 4.
Figure 4. Representation of the GAMBIT’S environment when the Dorr-Oliver Tank Configuration was imported from Inventor 10
Volume 1: Impeller: The reason for which we “break” the shaft into two parts is because we have that the rotational zone and everything that is inside itthis zone must stop where the interface stops, in order of the model to be functional for simulationng it in FLUENT. As a result in the CAD program we should add this piece of the shaft.
Volume 2: Rotational Zone (RZ): Not in actual geometry but needed for the simulation in FLUENT. In the MRF system the three- dimensional Navier – Stokes equations are solved unsteady while in the outside system the equations are solved steady state.
Volume 3: Piece of Shaft (small piece) which is inside the RZ: This is the small piece of the actual shaft that needs to be inside the rotational zone
Volume 4: The rest of the shaft (the large piece)
Volume 5: The rest of the tank
Steps for creating vVolumes that can be meshed without GAMBIT reporting the error “Can not be meshed because there is only adjacent cell”
a. Split Volume 5 using Volume 2 : In the
i. Operation menu in the left Column choose the first box (1st )
ii. Geometry menu choose the fourth box (4th)
iii. Volume menu choose the second box (2nd) from the second row (2nd ) , right click on it and choose: Split Volume
iv. Split Volume menu choose Volume 5 and Split it with (Volume Real) Volume 2 and delete the old one. From the choices you have:
Retain
Bidirectional
Connected
Choose the last one (Connected) and unclick the rest (they will become grey)
b. Subtract Volume 4 from Volume 5 : In the
i. The same as before (a. i.)
ii. The same as before (a. ii.)
iii. Volume menu choose the second box (3rd) from the first row (1st ) , right click on it and choose: Subtract
iv. Subtract Real Volume menu choose Volume 4 to be subtracted from Volume 5. Do not click any of the retain buttons.
At the end of this procedure we will have just two volumes, one for the rotational zone and one for the rest of the tank. In other cases we may end up with more than two volumes. This depends on how the initial geometry was constructedbuild up in the CAD program.
The next step after let’s say this “healing of the geometry is to set the Boundary Conditions in GAMBIT.
2. Setting the Boundary Conditions (BC) in Gambit.
From the Operation menu choose the third box (3rd) and from the Zone menu choose the first box (1st). This box is referred as the Boundary type command where one can specify different types of Boundary Conditions such as: Wall, Axis, Outflow, Symmetry, Periodic and others (In the Type menu). In continuation press in the Action menu the first choice on the left which is Add and type a name for the first BC. Then from the Face Menu choose all the faces from which the boundary consists of and press Apply. In case of mistakes there are in the Action Menu other choices to modify or delete the BC that are not valid. In our case we set everything as a Wall except from the faces that include the rotational zone which we set as an Interior.
After setting the above BC select the second box (2nd) of the Zone menu and set the two volumes (Volume 2 and Volume 5 in this example) as Fluid. This means that inside and outside of the rotational there is the working fluid (in our case is water but we will talk later on how we set this up in FLUENT).
3. Meshing the model in Gambit.
For the meshing choose the second box (2nd) of the Operation menu, the forth (4th) from the Mesh menu (this is for Volume meshing) and lastly choose one by one the existing volumes. In the next boxes there are some choices about the mesh elements. The menu includes the following choices:
a. Hex
b. Hex/Wedge
c. Tet/Hybrid
From which we select the last one (hybrid grid with tetrahedral and triangular elements).
The Type menu includes the following choices from which we choose the first (Map) and from the Smoothing menu choose None
a. Map
b. Submap
c. Tet Primitive
d. Cooper
e. Stairstep
Under Spacing there are three choices from which we choose the second (Interval size):
a. Interval count
b. Interval size
c. Shortest edge %
For every volume we change the spacing depending on how detailed we want to be the mesh. For example for the shaft we don’t need too much detail because there is nothing that we want to capture. On the other hand, the rotational zone and the tank is where we need a fine mesh because all the fluid phenomena happen there.
If there is a need to remove a part of the mesh first of all we choose the volume that we want to unmesh then we unclick the mesh button in the Mesh Volume menu and we enable the two other boxes with the names: Remove old mesh and Remove lower mesh. A snapshot of the meshed grid of the Dorr-Oliver Tank can be seen in Figure 5.
Figure 5. Representation of the Mesh made by GAMBIT for the Dorr-Oliver Tank Configuration
After finishing the meshing of the model we go to the Solver dropdown menu in GAMBIT and we choose FLUENT 5/6. Now we are ready to export the mesh by following the steps:
FileàExportàMesh à(Choose Filename and Folder)àAccept
Now we are ready to load it in FLUENT
When we double click the FLUENT icon it will open another one asking which version of FLUENT we want to run. The available versions are:
2d
2ddp
3d
3ddp
From which we choose the last one. The dp in both two and three dimensional means double precision for the results (accuracy of 16 digits behind the number)
Step 1:
FileàReadàCase…
In this step we read the .msh file which we export from GAMBIT.
Step 2:
GridàCheck Grid
FLUENT performs various checks to analyze the quality of the mesh and report everything in the console window.
Step3:
DisplayàGrid
Here we can display every surface of the model (impeller, shaft, tank wall and etc.)
Figure 6. Display panel showing the grid in FLUENT
Step 4:
DefineàModelsàSolver
Here we choose if we want steady or unsteady calculations as well as the velocity formulation (System of reference)
Step 5:
DefineàModelsàViscous
Here we choose the turbulent model and some other aspects of them. The three turbulent models that we used were:
a. The standard k-e model with standard wall functions and without changing anything in the model constants
b. The RNG k-e with enabled the option of Swirl dominated flow and changing the swirl factor at the value of 0.02 as well as choosing the enhanced wall treatment in the Near Wall Treatment menu
c. The Reynolds Stress model with Standard wall treatment and enabled the options of Wall Boundary conditions from the k equation and the Wall Reflection effects from the Reynolds stresses menu
Step 6:
DefineàOperating Conditions
Here we set the operating condition such as the gravity and condition for the pressure
It is important here to know how the axes have been set in the CAD program in order to know in which direction we should apply the gravity. In our example the z-axis is the perpendicular axis therefore in the Operating Condition menu we set as an operating pressure 101325 Pascal= 1atm at z=0.448 which is the top of the tank where the liquid stops and the gravity acceleration as -9.81 again in the z-axis because is pointing downward.
Step 7:
DefineàMaterials
At this point we will choose the working fluid which in our case is water. By default FLUENT uses air so we need to change it. In the following figure the materials menu can be seen.