Cfd_-_fluent_mar_2013.pdf

PRÁTICAS de ENGENHARIA QUÍMICA IV (CHEMICAL ENGINEERING PRACTICE IV)

Computational Fluid Dynamics Brief tutorial for Fluent and Application Exercises

February 2014

Have you wondered why the F117 stealth aircraft have flat, angular surfaces and looks like the flying diamond, while the B-2 stealth aircraft have aerodynamic rounded surfaces? Simply because the F117 was designed around 1975, when mainframes did not have the sufficiently large memory and the sufficiently powerful CPU to allow three-dimensional designs, or round shapes, and therefore when the radar cross section of an aircraft configuration could be accurately calculated only if it was in two dimensions. On the other hand, the B-2 was designed later using three-dimensional computations on vector supercomputers capable of hundred of megaflops. This i perhaps the most dramatic example of the impact of high-performance computing on engineering design, but not the only one. In Comput. Methods Appl. Mech. Engrg. 184 (2000) 143

Pedagogical Objectives After the execution of this work, the student should be able to: o Perform simulations at steady-state conditions with a commercial CFD program (Fluent), in order to characterize the flow hydrodynamics in a given system; o Perform simulations at transient state with Fluent in order to obtain the residence-time distribution (RTD) in a given system and, consequently, identify and quantify anomalies, particularly deadvolumes; o Perform simulations for other simple problems, at steady or transient state. Proposed work In the week after the execution of this work, you must deliver a record sheet of the results that should contain the following information (see section "Tutorial example - RTD determination in a lagoon", parts 1 and 2): o Figure with the time evolution of the outlet tracer concentration, in the dimensionless form (Danckwerts’ F curve); o Figure with the RTD; o Calculation of the mean residence time and of the dead volume fraction; o Figures of the tracer concentration contours inside the reservoir for different instants, representative of the problem under study.

In case you have to deliver a complete report or to perform an oral discussion for this work, it is also intended that you perform the complementary exercise described at the end of this manual, including in the report or in the documentation to present in the discussion the following information: o Table with the main conditions used in the simulations (inlet and outlet boundaries and corresponding fluid velocities); o Figure with the time evolution of the contaminant concentration in the outlet stream;

1

o Calculation of the contaminant mean fraction inside the lake at the final instant (t = 5×τ) and of the percentage of contaminant removed from it – you should clearly indicate the calculation procedure used. o Figure with the time evolution of the contaminant mean molar fraction in the lake, identifying the time at which it decays to 1% (at the initial instant this value was 5%). o Figures of the contaminant concentration contours inside the lagoon for different instants, discussing particularly the aspect of the space distribution at the final instant.

Introduction This tutorial intends to illustrate, with a simple example, some of the potentialities of the Fluent program, as well as some aspects that are important to take into account in order to obtain successful simulations. This commercial code of computational fluid dynamics (CFD) is very complete and has a wide applicability that covers several types of industries, such as: chemical, aerospace, automobile, biomedical, environmental, polymers processing, etc. (see www.fluent.com). It is aimed that students reproduce the steps described in this tutorial so that they familiarize themselves with the program. At the end of the tutorial a second exercise is proposed that should be also performed and whose results should be saved in a CD. This CD should be properly identified and delivered together with the report (or with the documentation to present in the discussion).

Tutorial example - RTD determination in a lagoon The mean residence time ( t r ), i.e., the time that the fluid elements spend, on average, within a certain reservoir or reactor, particularly in water treatment systems, has an important effect in its performance, since it affects the conversion of the biodegradable material. Besides that, the geometry of the reservoirs/biological lagoons, as well as the positioning adopted for the inlet and outlet streams, affect the residence-time distribution (RTD) of the fluid elements in the reservoir and, consequently, t r . In fact, this function (RTD, commonly represented by E(t)), gives us an idea of which fraction of fluid elements has spent a long or short time inside the reservoir, i.e., it is a distribution function, since the fluid elements will follow different trajectories in the system. A way of obtaining this and other "theoretical" functions is through the classic tracer experiments, of the stimulus-response type. I.e., a disturbance is made at the inlet stream (tracer injection by pulse input, by step input or by another way) and the system/reservoir response is measured at the outlet.

2

The information obtained allows also the diagnosis of reactors operation, modelling and prediction of the conversion (Rodrigues, 1981), as well as a more efficient design of water treatment units. So, tracer experiments are of extreme importance in these systems (or obtaining the RTD by other means). However, the mean residence times in these large reservoirs or lagoons are extremely high (from one day up to several months) (Metcalf & Eddy Inc., 1991), and therefore tracer experiments are impracticable. Possible strategies to overcome this problem are: i) to obtain the RTD in pilot-scale facilities, with several geometries, and scale-up the results obtained (this is however an expensive and slow process), or ii) to derive the RTD by solving the Navier-Stokes and diffusion-convection equations of the system considered (e.g., Brunier et al., 1984) (this is on the other hand a somewhat complicated process). The CFD commercial codes available (for instance Fluent, CFX, Fidap, Phoenics, STAR-CD, FLOW3D, etc.) solve those equations numerically, and thus the second approach will be adopted here. In the problem proposed, which considers a two-dimensional reservoir (biological reactor) with laminar flow, and which geometry will be described later in detail, you should perform the following tasks that are the main objectives of the present work: i) characterize the hydrodynamics in the reservoir and ii) determine the RTD from a tracer experiment, including also diagnosis of the system (characterization and quantification of the dead-volume).

Part 1 Simulation of the flow hydrodynamics The file that contains the grid1 to be used in this exercise (tracer.cas) may be obtained in the page of the course unit at SiFEUP. Save the file in your work folder, which you should create in the available computer. Run the Fluent software, previously installed in several computers of the room2. Start by choosing "2D" in Dimension, which is used to simulate two-dimensional flows, and choose “Double Precision” variables, in Options. Then, press OK. (Note: Given the high number of figures presented in this tutorial, and since they are clearly described in the text, we opted to not present the respective legends. Notice, however, that this procedure should not be adopted in your reports, i.e., all the figures presented in the reports should include an appropriate legend).

1

In fact, the grid is a computational representation of the system geometry in which the equations that characterize it will be solved. 2 Fluent may be run in any other computer of the FEUP network, for instance to conclude the work out of the schedule time of the class. This may be done through the applications server (http://apps.fe.up.pt/), which makes unnecessary the local installation.

3

Read the file that contains the grid (tracer.cas): File

Read

Case...

Note: It is worth noting that some of these windows may have a slightly different aspect from the ones here presented, due to the fact that another version of Fluent is now available. However, you should not forget to activate all the options presented, otherwise the numerical results obtained may be different!

4

We may start by performing a check of the imported grid: Mesh

Check

In the window some geometric parameters are presented that may be useful to check the grid quality. For instance, the maximum and minimum volume of the several elements that constitute the grid are indicated (control volumes), as well as the maximum and minimum values of the face areas that limit the several control volumes. The indication of a negative value for a control volume or for a face area is unacceptable, being thus possible, by this simple procedure, to check if the imported grid can or not be used in the simulation.

The grid used in this exercise has the following dimensions: 1m × 0.5m . The boundary that limits the computation domain was subdivided in 30 segments (each with a dimension of 0.1 m), being its numbering presented in the following figure. In this way, the grid may be used to simulate a variety of cases, being possible to choose different combinations for the system inlet and outlet locations. In the present exercise we will consider that the system (a lagoon, in our case) has an inlet stream (in

fronteira_1) and an outlet stream (in fronteira_17). All the 30 segments that constitute the boundary of the system were defined as walls in the grid generating program (Gambit). So, depending on the case to study, some of the segments will have to be redefined as inlet (velocity_inlet) or outlet (outflow). This procedure will be explained later on in detail.

5

(0, 0.5) 6

7

8

9

10

11

12

13

14

15 (1, 0.5)

5

16

4

17

3

18

2

19

1

y

20

x

(0, 0) 30

29

28

27

26

25

24

23

22

21 (1, 0)

The graphical visualization of the grid may be done using the following command:

Display

Mesh ... (Display)

If you wish to move the grid you may use the mouse left side button and drag it to the desired position. It is also possible to perform a zoom to the grid in order to analyze in detail a grid portion. For that, you should execute first the following command:

6

Display

Mouse Buttons

Next, a small menu is presented where the functions of each of the mouse buttons are indicated. You may change, for instance, the function of the mouse right button to "mouse-zoom."

This way it is possible to zoom-in and zoom-out using the mouse right button. To zoom-in you should press the mouse right button at the left upper point of the figure that you intend to enlarge and drag the mouse (continuously pressing the button) to the left lower point of the area that you intend to enlarge. Using this procedure it is possible to visualize with more detail a certain area of the grid, e.g. close to the left lower corner of the domain:

To zoom-out the image you should press the mouse right button and drag it in the NW direction, keeping pressed that mouse button. The less you drag the mouse with the button pressed, the large will be the degree of zoom-out (or zoom-in). Try it!

7

We will now define the flow regime for the problem in study. Because, in this case, the flow has a low Reynolds number, the regime is laminar, which is defined in:

Define

Models

“Viscous – Laminar”

The alternative flow types would be the ideal case of an inviscid fluid (i.e., of null viscosity irrotational flow) or turbulent flow regime (for which several approximate equations are available to model the turbulence; e.g., the k-ε model is frequently used in engineering calculations).

We will now define the fluid properties. For that, you should execute the command:

Define

Materials

agua

Create / Edit

As you can check by clicking in Fluent Database... in the menu that appears, Fluent has a database with several compounds, for which the relevant physical properties are pre-defined. Going back to the

Materials interface, you can verify that, in this example, two fluids (check in Fluent Fluid Materials) with equal physical properties were created: water and tracer. Water already existed in the Fluent

8

database (named water-liquid (h2o)). However, in order to simplify the data treatment, we defined a fluid with properties identical to water: ρ = 1000 kg/m3 and µ = 0.001 kg/m.s.

Let us now define the boundary conditions of this problem. To activate the respective menu you should execute the command:

Define

Boundary conditions

As mentioned above, all the 30 segments that delimit the computation domain are defined by default as walls. In the present example it is therefore necessary to change only segments 1 and 17 to inlet and outlet boundary conditions, respectively. The zone entitled "fronteira_1" corresponds to the region of the calculation domain through which the fluid enters into the reservoir, and so should be changed to a "velocity-inlet" type boundary.

9

It is necessary to define the inlet velocity of the fluid, which in the present example will take the value of 0.0001 m /s (“Magnitude, Normal to boundary”, Reference Frame - Absolute). In these conditions the Reynolds number, defined in terms of the inlet conditions, will be:

Re =

ρUH 103 ×10−4 × 0.1 = = 10 10−3 µ

(1)

where U is the average velocity at the inlet section, with dimension H. The zone entitled "fronteira_17" corresponds to the outlet boundary, and thus should be changed to "outflow":

10

The parameter Flow Rate Weighting indicates the fraction of the outlet flow rate that leaves the system through that boundary. In this case, and because there is only one outlet boundary, the fraction of the outlet flow rate at fronteira_17 will be 1. Since we are simulating the flow of an incompressible fluid it is necessary to define the working pressure in a point of the calculation domain, what can be done with the command:

Define

Operating conditions

In this case we will define (arbitrarily) that the pressure is 101325 Pa at the point with coordinates (0,0) (note that, since the fluid is incompressible, the numerical solution obtained is totally independent of the stipulated pressure value).

At this point we are practically able to run the simulation, needing only to choose the computation method to obtain the numeric solution. For that, you should execute the command: 11

Define

General

Automatically, the following menu will appear:

that allows deciding, among other aspects, if the numeric solution should be obtained by a transient process ("Transient") or iteratively ("Steady"). If we know in advance that we are in the presence of a transient flow, then it is imperative to use the "Transient" formulation to correctly predict the flow along time. If it is a steady flow (or if we are interested in the steady-state solution only) it will be preferable to use the "Steady" formulation.3 In the first part of this example, as we are studying the flow hydrodynamics at steady-state, the Fluent parameters presented by default, shown in the previous figure, should be adopted. To start the simulation it is necessary to initialize all the fields, what can be done with the command:

Solve

3

Initialization

Initialize

However, the “transient” formulation may also be chosen, being only of interest the final solution obtained at steady-state.

12

Let us start, for instance, from a null field of velocities and pressure; thus, we simply need to press the button "Initialize". It is important to follow the evolution of the residues along the iterative process (to easily check if the calculation is converging or diverging). You should therefore activate the command that makes the program to plot a chart with the residues of the several equations:

Solve

Monitors

Residual (select the Print option)

13

Edit

It is also suggested to reduce, in this menu, the convergence criteria of the several residues from 10-3 to 10-5 (see previous figure). This procedure aims to unequivocally guarantee that the iterative process for solving the linear equations systems, which result from the discretization of the transport equations, completely converges.

The sources of numeric error may arise from an insufficient refinement degree of the grid and/or from the numeric errors associated with the space and time (in the case of transient simulations) discretization schemes used. Without going into deep details, it is worth to refer that Fluent discretizes the several terms of the balance equations using centred differences, which have 2nd order precision. The exception occurs with the convective term of the equations, wherein the user should select the discretization scheme to be used, among the several possible options (First Order Upwind, Second Order Upwind, Power Law, QUICK and Third-Order MUSCL). The less precise scheme is the

backward differences (First Order Upwind) and one of the most precise is the QUICK one (it may reach 3rd order precision, being frequently of 2nd order). By default, Fluent uses the backward differences scheme (First Order Upwind) due to its high stability. However, and as reported in the literature, this discretization scheme should be avoided due to its low numeric precision. To minimize the numeric errors, you should select the QUICK scheme for the discretization of the equations’ convective term4. For that you should run the command sequence:

Solve

Methods

and select the option QUICK in the discretization of the convective terms of the momentum conservation equations:

4

One could also generate a new grid, more refined than that presently used. The disadvantage of this procedure is that as more refined is the grid, more computational time will be required to reach the solution.

14

Solve

Controls

Finally, we can start the simulation:

Solve Run Calculation ...Calculate indicating a reasonable number of iterations (e.g. 1000) to guarantee that the iterative process converges. To avoid unnecessary delays it is suggested to use a "Reporting Interval" of 10, for instance, meaning that the values are updated in the residues plot and in the Fluent´s interface only every10 iterations.

At the end of ca. 370 iterations (check it, otherwise you may have committed an error) an indication of convergence for the iterative process should be obtained.

15

Now that we have reached the intended solution, it is convenient to represent the numeric results in a graphical way. It is possible to generate "contour plots", as well as representations of the velocity vectors in the computation domain ("vector plot"), among others.

For demonstration purposes, the following examples are shown:

Display

Graphics and Animation Contours

16

or making a zoom near the outlet (and removing the option "filled"):

NOTE: The contour plots (or any other figure made with Fluent) can be exported to a text editor (e.g. Word). For that you should click with the mouse right button in the upper bar of the corresponding figure

starting by defining the properties (Page Setup...) intended for the image:

If you wish to export the coloured figure you should select the option Color. The option Reverse

Foreground/Backgroung allows changing the figure background from black to white, what is useful to avoid unnecessary ink consumption during paper impression. 17

To obtain charts with the velocity vectors you may run the command sequence:

Display

Graphics and Animation

18

Vectors

By default, a vector is placed in each cell of the calculation domain, what can difficult the understanding of the figure. The parameter Scale (1 by default) allows resizing the vectors, increasing (Scale>1) or reducing (0<Scale<1) its length. For instance, Scale=2 doubles the dimension of the reference vector, while Scale=0.5 reduces it to one half. The item Skip can also be useful, and it indicates the number (integer) of cells that are not considered between each two vectors represented in the figure; Skip=0 indicates that all the vectors are represented, while Skip=3 (for instance) indicates that between each two vectors shown in the figure, 3 vectors are not represented. In the next figure the use of these parameters is shown to better to illustrate the vectorial field close to the outlet boundary (Scale=2 and Skip=2 were used, and a zoom was done near the outlet).

By observing the velocity vectors it is possible to predict the trajectories followed by the fluid inside the lagoon/reservoir. A more efficient way of representing the stream lines consists in the representation of a contour plot of the stream function, what can be done with the following command:

Display

Graphics and Animation Contours

Although it is not obvious, in the previous figure it is possible to predict the existence of a high recirculation in the upper left corner of the domain. If you run again the command:

19

Display

Graphics and Animation Contours

but remove the option Auto Range, and select the stream function range between 0.01 and 0.01045688 kg/s, you will obtain the following figure:

where a recirculation is clearly visible (it corresponds to a dead volume in a chemical or biological reactor - confirm that in such area the velocities are reduced). It is also possible to identify two more small recirculations, in the upper right corner and in the bottom right corner of the domain, if the following ranges for the stream function are selected: Min=0.01 - Max = 0.01001 kg/s; and Min=0 Max = 7E-7 Kg/s, respectively). At this point it is convenient to save the results obtained (File Write Case & Data...), for instance with the name example 1 or part 1.

20

Part 2 - Simulation of a tracer experiment As mentioned above, not all of the fluid elements remain the same time within the lagoon/reservoir, and such information is condensed in a distribution function, the so-called residence-time distribution (RTD). To have access to that function, usually represented by E(t), it is common to perform tracer experiments, which is not more than a species that should be easily measurable at the reactor outlet (exhibiting as well other characteristics). We will now simulate a tracer experiment to analyze the system response to a step change in the inlet concentration, i.e., its concentration in the feed is suddenly changed, at the initial instant (t=0), from zero to a certain value, Co(t). Firstly it is necessary to define the new component (the tracer), with properties identical to water (to not affect the flow hydrodynamics inside the lagoon/reservoir); that component we will name "tracer." In this case, besides the numeric solution of the continuity and momentum conservation equations (Navier-Stokes equations), Fluent will have to numerically solve the transport equations of the chemical species. For that you should activate the Species Transport option, using the command sequence:

Define Models Species Transport & Reaction...

pressing “OK” will appear the follow window, please see in next page.

21

With the command:

Define Materials...

it is possible to confirm the presence of the "tracer" species, with physical properties identical to water5. Use the options indicated in the following figure for the calculation of the mixture properties, setting a value of 5×10-10 m2/s for the mass diffusivity (a typical value for liquids). At the end click in the Change/Create button, before clicking in Close.

5

Because the case file provided with this example had already pre-defined the species water and tracer, it was not necessary to define their physical properties.

22

Let us start by initializing the system containing water only, i.e., let us consider that for t=0 there is no tracer inside the reservoir (notice that we will make a step change in the inlet concentration):

Solve

Initialization

Initialize

This initialization originates a null field of velocities in the whole domain (see previous menu). It is therefore necessary to recalculate the steady-state solution for the situation in which the system is fed with water. Notice that this is done so that the velocity field is completely developed when the step change is performed in the inlet stream. For that you should confirm (or change in case it is necessary) that the water fraction in the feed stream (in this example at fronteira_1) is 1:

23

Define Boundary Conditions...

Let us now move to the simulation to compute the velocities field at steady-state conditions, for the case in which the system has only water:

Solve

Run Calculation

Calculate

keeping the parameter Number of iterations at 1000 and the Reporting Interval at 10. Again, after 370 iterations, the iterative process converges (for the tolerance previously set).

24

Let us pass now to the tracer experiment. The inlet boundary condition (in this example at

fronteira_1) should be changed because the feeding is no longer water and is now tracer: Define

Boundary Conditions...

The mass fraction of the species water should now be null, and the magnitude of the velocity vector should correspond to the desired value (in this case we will keep the value of the previous example, the one that corresponds to Re=10). Be aware that we only define the mass fraction of one of the species (in this case water), because the mass fraction of the other one (tracer) is obtained by the relation:

xtracer = 1- xagua . In a generic case that involves the transport of n chemical species, it is necessary to define the mass fraction of n-1 species.

25

During a tracer “experiment” the concentration of the tracer is measured at the outlet stream along time, Cs(t). This is an unsteady process, and that option must be activated:

Define

General …

by selecting the button "Transient" ,

Solve

Methods

In windowYou can activate the 2nd order implicit formulation (which is more precise). Similarly to what we have done previously, where the QUICK scheme was used to discretize the convective terms of the momentum conservation equations, we will also use it for the species, as illustrated in the following figure:

26

Solve

Controls

During the tracer “experiment” it is convenient to monitor the time evolution of the outlet stream composition, what can be done with the following command:

Solve

Monitors

Create

We will name this monitoring as "c-saida", being careful to activate the options indicated in the menu. Fill out the menu that appears after clicking in “Create”..., using the following parameters:

and press the "OK" button. 27

As you can see, we will monitor the tracer mass fraction at the outlet stream (in this case at

fronteira_17, but it can be at a different boundary, depending on the problem under study). In the same directory where you have saved the case & data files, a text file with the name c-saida.txt will be created, where the values of the tracer mass fraction will be stored along time (Flow Time). From such data it will be possible to determine the theoretical curves required for the following calculations: dimensionless system response (so-called Danckwerts’ F curve, F(t)), the RTD or E(t), etc., as referred below (see Eqs. (2), (3) and following ones).

To simulate the tracer experiment (now at transient state), select the command sequence:

Solve

Run Calculations

Calculate

A new menu appears where the time integration parameters are indicated:

For the current problem the space time is given by: τ=

V 1 × 0.5 × depth 5[m] = = Q 0.1 × depth × U U [m / s ]

Although the reservoir depth is unknown, this is not necessary for the calculations (it is a twodimensional problem) as shown in the previous equation. A reasonable estimate for the integration time interval (Time Step Size) will be ∆t = τ / 50 , i.e., for each space time, 50 time integrations are executed. The smaller the integration time interval, the greater will be the numeric precision, however 28

the calculation process will take longer. The use of ∆t = τ / 50 corresponds to a compromise between precision and computation velocity. For the present problem, we may use a value of 1000 s for the Time Step Size, corresponding to a fraction of 1/50 of the space time, τ = 5 × 10 4 s . The value of the parameter Number of Time Steps may be changed to 500, indicating that the tracer experiment will occur until θ = t / τ = 500∆t / 50∆t = 10 , i.e., until a time equivalent to 10 space times has been reached.

NOTE: Depending on the processor used in the simulation, this may be more or less time consuming. Typically, in an AMD Thunderbird© processor at 1GHz it will take ca. 20 minutes. It is advisable, therefore, to use computers with high clock speeds. The outlet tracer concentration versus time will take the form presented in the following figure6.

Do not forget to save again the simulation obtained (File Write ...), giving now a different name to the Case & Data file (e.g., example 1 part 2.cas or example 1 tracer.cas).

In the following figure, a representation of the tracer mass fraction contours is illustrated. It is important to note that for θ = 10 ( θ = t / τ ) the reservoir still contains some water, due to the stagnant zone previously identified.

6

Why does not the curve reach the value of 1? Is it possible to reach that value?

29

As mentioned before, during the simulation a text file is created containing the time evolution of the tracer mass fraction at the outlet stream (the file created may be easily edited using a spreadsheet program like MS Excel - use an empty space as the character delimiter for the columns7). From that file you can easily compute the Dankwerts F curve (Eq. (2))8. This will allow obtaining the RTD (Eq. (3)), the mean residence time (Eq. (4)), as well as to quantify the dead volume fraction (Eq. (5)) (Fogler, 1999; Rodrigues, 1981; Villermaux, 1993). It is intended therefore to quantify the dead volume fraction for the present example.9

F (t ) =

C s (t ) Co

(2)

E (t ) =

dF (t ) dt

(3)

∞

t r = ∫ t × E (t )dt

(4)

0

7

Additionally, in the computer control panel you should select “.” as the decimal symbol. Since the physical properties of both components (trace rand water) are equal, it is indifferent to calculate the tracer mass fraction at the outlet stream or its concentration. If you choose to calculate the concentration, later this will have to be normalized by the inlet concentration in order to obtain the intended theoretical functions, including the RTD. 9 To calculate the volume fraction corresponding to the dead, or stagnant, zone, you need to obtain the mean residence time 8

and to compare it with the space time. The tr is obtained from the E(t)curve, or E(θ),which should be integrated until infinite time. However, as suggested by Froment and Bischoff (1990), if an area of the recipient/reactor retains a portion of the fluid for a period of time greater than the mean residence time by an order of magnitude, then that zone may be considered as stagnant. Therefore, in the calculations of the mean residence time, you may truncate the integration superior limit at θ=10 (or t=10τ).

30

Vm t = 1− r V τ

(5)

Cs(t) is the tracer concentration at the lagoon/reservoir outlet at instant t, Co is the step width at the

inlet and Vm is the system dead volume.

The evolution of the tracer concentration contours inside the reservoir along time are also interesting to analyze, because they provide a good idea of how the concentration fronts evolve. For that you will have to simulate the process again and save some frames at different times. To better illustrate this transient phenomenon it is possible to execute animations in Fluent, although this is not demanded in this work. An example may be seen in the following site, in the Movie Gallery section: http://www.fe.up.pt/~mmalves/cfd/reactor/index.htm.

Complementary exercise In this second exercise, to be executed only if you have to present a report/paper or an oral discussion of the results for this work, we intend to study the best procedure to clean a reservoir that contains a high concentration of an undesirable compound. You should read the next problem description, in particular the notes at the end, before starting the simulation in Fluent. Suppose that the reservoir (e.g. a lake) contains a certain compound dissolved with a uniform concentration (consider an initial molar fraction of contaminant – tracer – equal to 5%). Admit that the lake is initially isolated (i.e., there are no inlet or outlet streams) (Solve

31

Initialization

Initialize…) ,

The purpose is to clean the lake by feeding it with clean water coming from two small streams, which course has been deviated (admit a zero concentration of the contaminant in those streams). The objective is to optimize the location of the inlet stream(s) and outlet stream(s), in order to, after a certain time, the largest possible amount of contaminant has been removed. As this study is time consuming, given the high number of possibilities, each group will only study one configuration, that consists of two water inlets and only one outlet (at a flow rate equal to the sum of the two inlet flows). Each group should study the configuration indicated in the following table:

Table 1 - Experimental conditions for the different groups. Week

1st lab session (week no. 3: starting at Feb. 24th) 2nd lab session (week no. 4: starting at Mar. 3rd) 3rd lab session (week no. 5: starting at Mar. 10th) 4th lab session (week no. 7: starting at Mar. 24th) 5th lab session (week no. 8: starting at Mar. 31st) th 6 lab session (week no. 9: starting at Apr. 7th) 7th lab session (week no. 12: starting at Apr. 28th) 8th lab session (week no. 15: starting at May 19th)

Conditions * st

nd

1 Inlet: 8; 2 Inlet: 3; Outlet: 12 (group 1); 1st Inlet: 10; 2nd Inlet: 26; Outlet: 3 (group 2); 1st Inlet: 16; 2nd Inlet: 2; Outlet: 20 (group 3) 1st Inlet: 19; 2nd Inlet: 12; Outlet: 7 (group 1);

Average velocity at

1st Inlet: 29; 2nd Inlet: 7; Outlet: 20 (group 2);

section 1 inlet:

st

nd

1 Inlet: 5; 2 Inlet: 1; Outlet: 18 (group 3)

0.025 m/s;

1st Inlet: 6; 2nd Inlet: 30; Outlet: 18 (group 1);

Average velocity at

1st Inlet: 15; 2nd Inlet: 21; Outlet: 3 (group 2);

section 2 inlet:

1st Inlet: 30; 2nd Inlet: 28; Outlet: 14 (group 3)

0.075 m/s

1st Inlet: 1; 2nd Inlet: 30; Outlet: 16 (group 1); 1st Inlet: 8; 2nd Inlet: 23; Outlet: 3 (group 2); 1st Inlet: 20; 2nd Inlet: 1; Outlet: 10 (group 3) 1st Inlet: 8; 2nd Inlet: 3; Outlet: 12 (group 1); 1st Inlet: 10; 2nd Inlet: 26; Outlet: 3 (group 2); 1st Inlet: 16; 2nd Inlet: 2; Outlet: 20 (group 3) 1st Inlet: 19; 2nd Inlet: 12; Outlet: 7 (group 1); 1st Inlet: 29; 2nd Inlet: 7; Outlet: 20 (group 2); 1st Inlet: 5; 2nd Inlet: 1; Outlet: 18 (group 3) 1st Inlet: 8; 2nd Inlet: 3; Outlet: 12 (group 1); 1st Inlet: 10; 2nd Inlet: 26; Outlet: 3 (group 2);

Average velocity at section 1 inlet: 0.050 m/s; Average velocity at section 2 inlet: 0.050 m/s

1st Inlet: 16; 2nd Inlet: 2; Outlet: 20 (group 3) 1st Inlet: 13; 2nd Inlet: 23; Outlet: 5 (group 1); 1st Inlet: 5; 2nd Inlet: 26; Outlet: 17 (group 2); 1st Inlet: 20; 2nd Inlet: 22; Outlet: 5 (group 3)

* ”group 1” refers to the Tuesday class, “group 2” refers to the Wednesday and “group 3” refers to the Thursday class.

32

Admit that the clean water feeds start at instant t0. It is intended to monitor the evolution of the contaminant concentration (consider the tracer species defined in the previous example) at the outlet stream along time. In this way, and performing a mass balance at transient state, it is possible to determine the mean concentration of contaminant inside the lake, at any instant. Do the calculation until a final time corresponding to five space times is reached.

NOTE: In order to make this example physically realistic, you should resize the geometry for the following dimensions: 1000 m x 500 m. Since the original dimension of the geometry was 1 m x 0.5 m (problem 2D), you should then enlarge 1000 times the dimension of the initial grid at “Scaling Factors”:

Mesh

Scale

Press Scale!

As the values of the Reynolds number are very high, the flow is in turbulent regime, and you should execute the command: Define

Models

Viscous-Laminar

and select, e.g., the k-ε model option (use the Fluent default parameters). Do not forget that this will be a transient state simulation and 2nd Order implicit :

Define

General

33

Solve

Methods

Do not forget to monitor the contaminant concentration (tracer) with time at the outlet section...

Solve

Monitors

34

Create

Depends on the case studied

For the several conditions presented in Table 1, the space time is 50 000 s (13.89 hours). An acceptable value for the integration time interval (time step) is, e.g., 500 s. For this time step value you should execute 500 time steps (number of time steps) in order that the simulation finishes precisely at a time corresponding to five space times.

The results should be presented and discussed in the way you find more convenient (include with the report a CD with the Case & Data file(s) of the final results obtained in the simulations). Also include in the CD a summary of the conditions used in the simulation. This can be done using the command

Report

Input Summary

and selecting all the fields:

35

Although the execution of animations is not mandatory, it is suggested that for one of the simulated cases, at transient regime, you stop the simulation at different times, in order to obtain images that illustrate the time evolution of the concentration front.

Good work!

Bibliographical references Brunier, E., A. Zoulalian, G. Antonini, and A. Rodrigues (1984). “Residence time distributions in laminar flow through reservoirs from momentum and mass transport equations”, in ISCRE8 – The 8th International Symposium on Chemical Reaction Engineering, IChemE Symposium Series, Nº 87, 439-445. Fogler, H. S. (1999). Elements of Chemical Reaction Engineering, 3rd ed., Prentice-Hall. Froment, G.F., and K.B. Bischoff. (1990). Chemical Reactor Analysis and Design, 2nd ed., John Wiley & Sons, New York. Metcalf & Eddy Inc. (1991). Wastewater Engineering: Treatment, Disposal, and Reuse, revised by Tchobanoglous, G., and F.L. Burton, 3rd ed., McGraw-Hill, New York. Rodrigues, A.E. (1981). Theory of residence time distributions, in Multiphase Chemical Reactors, Rodrigues, A.E., J.M. Calo, and N.H. Sweed (Eds.), NATO ASI Series, Sijthoff Noordhoff, No. 51, Vol. I, 225-284. Villermaux, J. (1993). Génie de la Réaction Chimique – Conception et Fonctionnement des Réacteurs, Tec & Doc – Lavoisier, Paris.

36