Discovery Laboratory. Multiphase Flow. Pilot Plant 101. Author: Yujie Zhao, Jayanth Ganapathy, Sam Cockman. Academic Contacts: Colin Hale, Omar Matar

Transcription

1 Discovery Laboratory Multiphase Flow Pilot Plant 101 Author: Yujie Zhao, Jayanth Ganapathy, Sam Cockman Academic Contacts: Colin Hale, Omar Matar 1. Learning Objectives To examine the available literature on bubble drift velocity as a function of bubble dimensions, pipe diameter and inclination and fluid properties. To gain an appreciation of the importance of inertial, viscous, surface tension and buoyancy forces on the bubble rise velocity in a pipe. To use this methodology in conjunction with experimental results (generated as part of this laboratory project) and appropriate literature correlations to develop an approach for scaleup to industrial size pipeline systems. To establish a clear connection with the relevant fundamental fluid mechanical principles established as part of the Transport Processes modules in Years 1-3. To acquire working knowledge of computational fluid dynamics software in order to simulate the bubble rise process for a range of system parameters. To gain an appreciation for the impact of bubble rise processes in industrial applications such as gas lift systems in deep-water oil-and-gas pipeline riser networks. 2. Industrial Relevance Figure 1: Schematic of a gas lift system (reference?) Multiphase Flow Page 1 of 11

2 Gas lift is one of a number of processes used to artificially lift oil from wells where there is insufficient pressure within the reservoir to produce fluid from the well (see Fig. 1). The process involves injecting gas through the tubing-casing annulus to aerate the fluid and reduce its density. The reservoir pressure is then able to lift the oil column and forces the fluid out of the wellbore. Gas may be injected continuously or intermittently, depending on the characteristics of the well and the arrangement of the gas-lift equipment. As oil is recovered from more remote fields that are located further away from land in increasingly deep water (sometimes as deep as 1-2km) the ability to economically recover oil is increasingly subject to the successful implementation of riser base gas lift systems. As bubbles rise from the bottom of the riser pipeline to the platform or Floating Production, Separation and Offloading (FPSO) vessels, they may expand due to the very large differences in hydrostatic pressure from the bottom to the top of the pipe. This can affect the rate at which oil is lifted out of the riser system and may present significant challenges for control of separation equipment on the receiving facilities. Fundamental examination of the bubble rise process on a smaller scale system provides insight into the flow behaviour in these much larger pipeline systems through appropriate scaling laws. 3. Scientific Foundation In two-phase gas-liquid flow, the bubble flow pattern is characterised by a suspension of discrete bubbles in a continuous liquid, and has numerous flow regimes. (O.K. Matar, 2013) Void fractions (the ratio of gas volume to total fluid volume) may range from the extreme case of a single isolated bubble to that of a foam containing less than 1% of liquid by volume. Interactions between the forces that are due to surface tension, viscosity, inertia and buoyancy produce a variety of effects which are quite often evidenced by different shapes and trajectories. The regime in which bubbles are so large that they assume a cylindrical shape and almost fill the duct in which they are flowing is called intermittent flow. 3.1 The rise velocity of single bubbles The dependence of the rise velocity of a single bubble in vertical pipes (see Fig. 2) was first determined by Davies & Taylor (1949). Their correlation is shown below: d 1 2 u 0.35 gd (1) The validity of this equation was found to be correct by subsequent research for negligible viscosity, and for sufficiently large bubbles for which surface tension effects are weak. However, current offshore pipeline systems handle fluid with a wide range of temperature dependent fluid properties which may not be well described by Eq. (1). Multiphase Flow Page 2 of 11

3 Figure 2: A picture of a Taylor Bubble in a vertical pipe taken from Davies & Taylor (1949) Subsequent work for horizontal pipelines was done by Benjamin (1967) and he derived a correlation for the rise velocity of a bubble in horizontal pipes. It is as shown below: u d gd 2. (2) In the same way as the previous correlation, this only works when surface tension and viscosity effects are negligible. Although there has been a significant amount of research on vertical and horizontal pipes, there is very little data for the effect of inclination on bubble rise. A simple correlation that uses vertical and horizontal velocities to derive the predicted velocity at an angle was formulated by Bendiksen (1983) as shown below for F r< 3.5: 2 u 054. gd cos 035. gd 2 sin (3) d 1 1 Given a scenario where the horizontal velocity is 0 m/s, then Kabir & Hasan s (1986) equation below can be used to find the predicted velocities for different inclinations. Multiphase Flow Page 3 of 11

4 u d 1 gd sin 1 cos (4) In order to investigate the effects of bubble propagation over a wide variety of conditions, the relative contributions of inertial, viscous, surface tension and buoyancy terms need to be investigated. The dependence of the bubble motion on these forces is commonly characterised by the dimensionless groups listed in Table 1. Table 1: Definition of relevant dimensionless groups. Number Equation Bubble Froude number Fr b u d gd Morton number Eotvos number g Mo 4 L 3 L D 2 Eo Lg L 4. Experiment 4.1 Equipment Description The Bubble Rise Apparatus shown in Fig. 3 consists of several parallel 2m long tubes ranging in diameter from 0.004m 0.063m, mounted on an inclinable frame. An inclinometer has been fixed onto the equipment to ensure that the angles of inclination are accurate. The fluids used in this experiment are various mixtures of glycerol-water solutions giving viscosities ranging from approximately 1cP to 1100cP. All fluids must be handled within the confines of the drip trays provided. Measuring tapes have been fixed on the sides of the equipment to allow for accurate measurements of length. Before the experiments are carried out, ensure that pipes are fixed in place. If any pipes are found to be loose, please inform the demonstrator immediately. Furthermore, the equipment also has a collection tray attached to the bottom. The liquid collected here can be drained out using the tap at the front of the drip tray, which facilitates its recycling. Multiphase Flow Page 4 of 11

5 32 mm 4 mm Locking Handle 2 Locking Handle 1 Collection Tray Drip Tray x Figure 3: Photo and schematic representation of equipment. The pipe ID increases from 4mm to 63.5mm from the right to left of the picture. 4.2 Risk Assessment The Bubble Rise Apparatus is located in the pilot plant and so wearing PPE and a hard hat while operating it is mandatory. Visually check fittings before filling the test section with liquid to prevent leaks. Electrical equipment: Ensure power cables are secured, electrical testing is current and leaks are resolved. Moving parts: Ensure that all gaps are clear while modifying the inclination. Ensure any glycerol solution spilt on the floor is immediately cleaned to prevent the occurrence of slippery conditions. Chemical handling: Water and Glycerol Solutions are non-hazardous. PPE must be worn as described in Table 2. Table 2: MSDS data of used chemicals. Products Cas No. Safety Measure Properties Water Wear safety glasses and gloves Glycerol Wear safety glasses and gloves Non flammable, colourless liquid Boiling point = C Non flammable, colourless liquid Boiling point = C Multiphase Flow Page 5 of 11

6 For further information, please refer to the separate asset register and risk assessment documents. 4.3 Lab Procedure Familiarise yourself with the literature and the equipment Compile an experimental plan and timeline for two weeks of experimental work to examine the effect of various system parameters on bubble rise velocity, and get the approval of your demonstrator/academic contact. Determine the physical properties of various glycerol- water solutions. Key properties are fluid density, surface tension and viscosity Preparing solution L containers are used to prepare the required solutions for the experiment. 2. These containers are heavy and so care should be taken when handling them. If necessary, ask for help to move these. 3. The weighing scale (25 kg) should first be kept in a drip tray. 4. The empty 25 L container should then be placed on the weighing scale. 5. The required amount of Glycerol should be added first, with the aid of a funnel, before the appropriate amount of water is added to get the solution up to the required concentration. 6. It is up to you to decide the quantity of each solution to be prepared. 7. Glycerol can be found in 5 L/25L containers at the loading area. Water can be used from the sink. Distilled water is not required for this experiment Bubble Rise Equipment 1. Incline the test section to an angle of roughly 60 to the horizontal. 2. Ensure that the bottom cork is tightly closed to prevent leakage. 3. Using an appropriate funnel, fill the pipe with the necessary solution until the pipe is almost full. Leave a small gap so as to enable the top cork to be closed. 4. Close the cork tightly on the top pipe. 5. Adjust the inclinometer to the necessary angle. 6. Unlock the equipment using the handles on each side of the tilting table. 7. Adjust the equipment to the appropriate angle. This is done by ensuring that the bubble in the small level measure is situated between the 2 dark green areas. 8. Lock the tilting table in place by locking the handles. 9. Bubbles are produced by removing the cork at the bottom and quickly replacing the cork once a bubble is formed. By adjusting the time for which the cork is removed, you can adjust the bubble size. 10. Velocity of the bubble is calculated by measuring the time the bubble takes to travel between two designated points using a stopwatch and then dividing the distance by the time. 11. This process should be repeated multiple times to ensure precise measurements of velocities. 12. Once all measurements are done for a given solution, the collection tray at the bottom can be emptied by opening the tap and letting the solution out into a beaker/drum. This can also be done during the experiment so as to reuse the solution, preventing the need to prepare excessive quantities of solution. 13. The equipment must be totally rinsed with water and wiped clean before the experiment is run again with a solution of different glycerol composition. Otherwise, your results could be Multiphase Flow Page 6 of 11

7 compromised Data Analysis 1. Determine the predicted bubble rise velocity for the specified inclination angles and liquid viscosities using appropriate correlations from literature. 2. Produce appropriate plots of fluid properties as a function of temperature for each glycerolwater solution used. 3. Study these plots thoroughly and observe how liquid properties change with temperature. 4. Produce appropriate plots of bubble drift velocity as a function of diameter and inclination angles for different fluid compositions. 5. How well do the predicted and measured bubble rise velocities agree? 5 CFD Modelling 5.1 Numerical Simulation Setup In order to carry out numerical simulations of the bubble rise problem, the computational fluid dynamics (CFD) package ANSYS Fluent 14.5 will be used. This package provides numerical solutions to the equations of mass and momentum conservation, governing the flow of the gas bubble and surrounding fluid. These solutions allow us to visualise the bubble motion and associated velocity and pressure fields throughout the computational domain. Note that heat transfer effects have been neglected in the present study; hence, numerical solutions of the energy conservation equation will not be provided. To model the air bubble motion in the fluid-filled tube, the interface between the two phases will be tracked using the volume-of-fluid method. The interface location is recorded by introducing a variable, called the volume fraction, whose value is determined via numerical solution of an additional equation to the mass and momentum conservation equations: the volume fraction equation. A key advantage of the use of CFD is the ability it affords us to examine the complex dynamics involved in fluid flows (particularly multiphase flows) very closely, and to extend the knowledge acquired based on experimental data to cases that would otherwise require extensive work developing new experimental apparatus and data-collection procedures. An example of the results obtained via CFD simulations is provided in Figure 1. Some of the possible objectives of this discovery laboratory project are therefore the following: To elucidate the growth and departure of Taylor bubbles from the tube inlet using CFD simulations. (The report tools in FLUENT allow for a detailed analysis of the fluid properties at incremental time steps.) To replicate a subset of the experimental observations using CFD simulations (whilst keeping in mind the time-constraints associated with this Discovery laboratory project). To examine the difference between the results obtained based on two- and three-dimensional simulations in order to assess the importance of non-axisymmetric effects. To examine the influence of parameter ranges on the dynamics of bubble rise that have not been studied in the literature. Multiphase Flow Page 7 of 11

8 Above: 3D simulation Water Inclined Left: 3D simulation Glycerine Vertical Right: 3D simulation Water Vertical Below: 2D simulation Water Inclined Figure 1 Still images from various examples of CFD simulations in both 3D and 2D. Red indicates the air phase (bubble) and blue the liquid phase (stagnant Fluid) 5.2 CFD Simulation Procedure Mesh Generation in ICEM CFD The ICEM CFD software package developed by ANSYS should be used to generate the geometry and mesh for the simulations. Detailed guidance for the construction of a mesh is given in Appendix 1, but the general procedure is as follows: 1. Create the geometry using points, curves & surfaces. Multiphase Flow Page 8 of 11

9 2. Block the surfaces this allows specification of the number/distribution of nodes along curves 3. Generate the mesh 4. Define parts 5. Export the mesh as a.msh file to be used in FLUENT ` Solution Setup in ANSYS FLUENT Launching ANSYS FLUENT opens the following launcher window. The appropriate dimension should be selected, along with the double precision checkbox (increasing accuracy of solution). Serial processing utilises a single process, whilst parallel processing speeds utilises a number of processes simultaneously. Detailed guidance for simulation setup is included in Appendix 2. Figure 2 The Ansys FLUENT launcher window. The following should be displayed in the console and graphics window when the simulation is running. Figure 3 the console and graphics window when simulation is running. Multiphase Flow Page 9 of 11

10 5.2.3 Data Analysis in ANSYS FLUENT or CFD-Post Once the simulation has been completed, you can visualize the results using an embedded postprocess tool to plot the velocity field and vapour volume fractions. Again, this is discussed in further detail in Appendix 2. CFD-Post (developed by ANSYS) can also be used for a more in depth analysis of a FLUENT case. It is also possible to read multiple data files for the same case, to study and analyse multiple time steps (data files) simultaneously. CFD-Post can be launched from the start menu. 6 Dissemination and Feedback Plan for Experiment (Place Holder) In advance of the experiment, you need to perform a literature search to familiarise yourself with the subject and a risk assessment. You will also have to compile a plan for two weeks of experimental work. All three will have to be submitted per group at least 1 week before labs start and will be assessed by the academic contact. During labs you will need to keep individual lab notebooks, which will be reviewed and marked by the demonstrator. Your personal, practical and safe working skills will also be assessed. In agreement with the demonstrator or lecturer, each group should prepare the following: A report of no more than 10 pages in length (not including appendix) Ensure that each contains: An executive summary An introduction explaining the motivation and the relevance of your work An experimental section describing your equipment and procedure Diagrams and/or tables of the data collected Sample calculations Possible sources of errors and error analysis A discussion section with a critical evaluation of your results An outlook with ideas for improving the experiment The report will be assessed by the academic contact and discussed in a group feedback session. An overview of the Discovery Lab assessment is shown below: Full details of assessment criteria and deadlines can be found on Blackboard. Multiphase Flow Page 10 of 11

11 7 List of Symbols d Bubble diameter. m D Pipe diameter. m Eo Eotvos number - Fr b Bubble Froude number. - g Acceleration due to gravity. m/s 2 u d Weighted mean drift velocity of the gas phase relative to the liquid. m/s Y Viscosity-surface tension number - L Dynamic viscosity of the liquid. Ns/m 2 G Gas density. kg/m 3 L Liquid density. kg/m 3 Surface tension. N/m 8 References 1. Matar, O.K., 3 rd Year Fluid Mechanics Lecture Notes, Department of Chemical Engineering, Imperial College London (2013) 2. Davies R.M. & Taylor G.I. (1949) "The mechanics of large bubbles rising through extended liquids and through liquids in tubes.", Proc. R. Soc., Vol. 200A, pp Hewitt G.F. (1982) "Gas-liquid two-phase flow,", Chapter 2, Handbook of Multiphase Systems, edited by G. Hetsroni, Hemisphere Publishing Corp. 4. Wallis G.B. (1969) "One dimensional two-phase flow.", New York, McGraw-Hill, White E.T. & Beardmore R.H. (1962) "The velocity of single cylindrical air bubbles through liquids contained in vertical tubes.", Chem. Eng. Sci., Vol. 17, pp Brown RA.S. (October, 1965) "The mechanics of large gas bubbles in tubes: 1. Bubble velocities in stagnant liquids.", Can. J. Chem. Eng., Vol.43, pp (1965). Multiphase Flow Page 11 of 11

12 Discovery Laboratory Multiphase Flow - Appendices 1. Creating a Mesh 1.1. What is a geometry? The geometry used in a CFD simulation defines the problem domain and boundaries; it is the area (2D) or volume (3D) containing the fluids of interest. Boundary conditions can be assigned to the edges or surfaces outlining the geometry What is a Mesh? CFD relies on the discretisation of equations governing the state of fluids within the computational domain. Meshing a geometry allows the computational domain to be split into numerous elements/cells, within which the discretised equations can be solved. The piecing together of these individual elements gives a complete picture of the fluid flow, at a point in time. In a transient solution such as bubble rise, these elements can be solved repeatedly to show how the flow develops over time. An example 2d mesh is shown below: Figure 1 - an example 2D mesh of a curved pipe section. We note that in addition to space, time is also divided into discrete time-steps. Choosing the size of the time-step is of crucial importance and is related to the choice of spatial grid-size. Generally, in order to increase accuracy, one must refine the spatial grid, which then reduces the stability of the numerical scheme leading to the generation of spurious results (i.e. numerical artefacts that have no physical analogue). Remedying this issue involves the reduction of the time-step, which on the one hand alleviates the stability problem, but on the other hand, leads to longer computational times Some Meshing Terminology Element/cell - one discrete small subsection of a computational domain.

13 Time-step a discrete unit of time, the length of which varies according to various mesh and setup parameters. A series of time steps in the result of discretising the time dependent terms of the equations governing the fluid flow. Node a vertex of an element/cell. The location/number of nodes are often considered when meshing as opposed to elements. Mesh Quality - affects both the accuracy of the CFD solution and the computing power required to reach a solution. Structured Mesh consists of a regular arrangement of quadrilateral (2D) or hexahedral (3D) elements. This is usually achieved through blocking, and often requires less computational resources than unstructured meshing Blocking - a series of quadrilateral or hexahedral blocks can be introduced around the geometry. Each edge on a block can be split into a specified number of points, and associated with an edge on the geometry these points will define the number of cells along each edge of the geometry. In essence, this allows a structured grid to be defined, and distorted to non-rectangular geometries such as pipes. Unstructured mesh consists of irregular elements connected in a non-uniform manner. Can utilise any shaped element. They tend to require more computational power than structured meshes due to the inability of the solver to easily create regular arrays from the irregularly spaced elements 1.4. How to create a structured 2D mesh in ICEM CFD Shown below is the main ICEM CFD display upon launching the software, with the curved pipe section geometry shown above. Tabs Options Console Graphics Window

14 1) Create the geometry - Construct the boundaries of the solution domain (pipe) using points and curves within the geometry tab in ICEM CFD. At this stage, consider the pipe diameter to be studied, and the appropriate pipe length (given the flow dynamics under investigation). Create a surface from the boundary curves only defined surfaces are meshed in ICEM CFD. 2) Block the surface - Within the blocking tab, use the create block option to create a 2D block from the surface. The pre-mesh params option allows for edge parameters for the block to be defined. Consider both uniform distribution of points, and distribution according to different mesh laws. Before proceeding, associate block edges with the appropriate geometry curves. 3) Generate the mesh - Once the pre-mesh parameters are defined, the mesh can be computed by right-clicking Pre-mesh in the top left panel of ICEM, and clicking recompute. Clicking convert to unstructured mesh will then produce a visible mesh. 4) Define parts for future application of boundary conditions - Right clicking Parts in the top left pane of ICEM allows the creation of parts. This enables the mesh to be split into zones consisting of edges or surfaces. Later, this is useful for the assignment of different boundary conditions to different parts of the mesh. Consider the required boundaries for bubble rise simulation. 5) Export the mesh to a.msh file - Within the output tab, ensure the file is setup for ANSYS FLUENT, and use the write input option to create an appropriately names.msh file. In FLUENT, this can be opened directly How to create an unstructured 2D mesh in ICEM CFD 1) Create the geometry as above. 2) Setup mesh parameters - The objective here is to control the mesh density through adjustment of the maximum and minimum element size. Within the mesh tab, use the part mesh setup option to adjust and apply the mesh parameters. 3) Compute and generate mesh - Use the generate mesh option within the Mesh tab to compute the surface mesh. Some parameters can be experimented with here. 4) Define parts and export the mesh as above Extending the above instructions to 3D domains 3D geometries tend to begin with a series of curves in 2D, which can be modified to produce a 3D surface using the create/modify surface option within the geometry tab. Various options are available for experimentation. Once the desired 3D surface has been produced, blocking can commence as above, but with a 3D bounding box. Whilst blocking with just a 3D bounding box produces a usable pre-mesh, of particular use in pipe flow is the 0-grid tool in the split block option within the blocking tab. Applying an o-grid block to the relevant face splits the bounding block into an array of blocks with new corresponding edges. Experimenting with the transform blocks options to adjust the block size and distribution gives greater control over the element shape and density within the mesh.

15 Above left: a body-fitted grid. Above right: an o-grid The method for defining parts and outputting usable mesh files is comparable to the 2D instructions. Care should be taken to ensure the mesh is output as a 3D.msh file What makes a good mesh for 2 phase flow? Considerations. Sufficiently high mesh density to capture liquid films, vapour-liquid interphase & boundary layer effects a low-resolution mesh may also give an inaccurate solution in areas where there is a significant change in flow characteristics or fluid properties across a small distance. Locally increasing the element density is referred to as mesh refinement. Conversely, a lower mesh density should be used where applicable/possible The point at which refining the mesh has no impact on the given solution is referred to as mesh independence. Refining the mesh beyond this point increases simulation time for two reasons: o It increases the number of elements for which the governing equations need to be solved at each time step. o It reduces the time step size accordingly, since by rough approximation: time step = minimum grid size / maximum velocity in domain i to achieve the same stability & solution accuracy. A max element aspect ratio of 5 this refers to the ratio of length/width in a quadrilateral element for example. Higher aspect ratios lower the mesh quality, increasing computational time. The ideal is 1. A skewness of <0.85 ii the definition of skewness varies depending on the elemental shape, but in general, a skewness closer to 0 increases the likelihood of obtaining an accurate solution and prevents divergence of a simulation. A smooth transition from smaller to larger elements this reduces the probability of an erroneous calculation in an element.

16 2. Guidance for Problem Setup (FLUENT) 2.1. Solution Setup General The relevant parameters are: Navigation Pane Task Page Graphics Window Console Gravity allows angle of inclination to be specified without changing the mesh Time 2.2. Solution Setup - Models Multiphase Model see hand-out for details. Viscous Model this is key to the manifestation of phenomena observed in the lab. Model k-epsilon. K-epsilon model Standard. Others default Solution Setup - Materials This section requires specification of the fluids present in the simulation. FLUENT s database contains basic fluid properties for numerous fluids, but the user can also create new fluids and input the relevant properties Solution Setup Phases This section considers the discrete phases to be used in the simulation, and interactions between them. Of particular relevant to two phase bubble rise is the influence of surface tension and wall adhesion on flow characteristics, both of which should be addressed here. Ensure the phase material is correctly specified for both the primary and secondary phase.

17 2.5. Solution Setup Boundary Conditions The boundary conditions specified in a model have a significant impact on the final solution, as well as how closely the bubble formation agrees with literature and experimental findings. Factors addressed her should include Boundary condition type Fluid contact angle at the wall especially relevant in setups where it is anticipated that the liquid/vapour interphase will intersect with a wall. The turbulence specification method for each boundary recommended K and Epsilon (Default values) 2.6. Solution Setup Dynamic Mesh Perhaps not a mandatory part of the solution setup, but can be used if desired. Contains useful option which may help automate the simulation process. Only the Events button needs to be addressed in this section ensure the event is defined and on Solution Solution Methods In the section, the solution algorithms FLUENT uses to obtain a solution can be selected. The appropriateness of a solution method is depended on the models used, whether the solution is transient or steady, and the type of fluid flow under consideration. In our case, the default values for spatial discretization are applicable, but could be experimented with. Non-iterative Time Advancement should be applied. The appropriate Pressure-Velocity Coupling is flexible and should be researched. iii 2.8. Solution Solution Controls The default values are satisfactory for this case, but can be adjusted if the simulation is struggling to converge. iv The purpose of these relaxation factors should be known. Altering the relaxation factors can cause the simulation to take a lot longer to converge Solution Solution Initialisation & Patching Patching refers to the manual alteration of an element or region s properties. It enables the elements in a domain to have an initial condition before the simulation begins, as well as the boundaries. Of specific interest in the case of bubble rise is the patching of fluid volume fractions into the domain. From the top navigation bar, selecting Adapt > Region allows a region to be marked, onto which a volume fraction of the secondary fluid can be patched through Solution Initialisation > Patch. By default, the domain is filled with the primary fluid (Air) of volume fraction 1. Patching different shapes to the inlet of the tube may affect the ease of bubble formation. The region adaptation window

18 2.10. Solution Calculation Activities The patching window This pane allows the capture of solution animations and case/data files at regular time step intervals. The location of these saved files can be selected, allowing different folders to be specified for different simulations. Considering the limited available storage space, it is important to bear in mind the anticipated size of your data files & auto save frequency. The following commands are of great use when capturing images of phase distribution in 2D simulations at regular time step intervals: The simulation time step (incremental change in time after 1 solution iteration) should be specified here. The appropriate time step is related to the mesh density and quality, as well as the desired degree of solution accuracy, which is characterised by the courant number. An appropriate value for the courant number should be selected/obtained through suitable time stepping. Figure 2 - Command window within calculation activities pane. These settings capture a 2D image of the volume fractions across the entire domain.

19 2.11. Solution Run Calculation Fixed Time Stepping allows the time step to be fixed and the courant number to be varied accordingly. Variable Time Stepping allows the courant number to be fixed and the time step to be varied accordingly. Useful if abrupt changes in flow conditions are expected or a dynamic mesh is in place. The Calculate will begin your simulation, saving auto-saves in the specified folder Report These tabs allow the user to visualise the velocity field, phase distribution and other properties of the fluid across the domain, for the current time step. New surfaces can be created within the graphics panels, allowing for a 2D plane within a 3D domain to be studied.

20 3. Troubleshooting and useful links 3.1. Common Issues My fluids are behaving strangely at the interphase Lower the courant number to maintain stability Reconsider boundary conditions incorrect boundary conditions can create unphysical behaviour. My time step is very low Consider coarsening the mesh in areas where low detailing is necessary and velocities are low. If the simulation is stable and results seem physical, increase the courant number perhaps run these two simulations side by side to ensure there is no variation in the solution. Each iteration is taking a very long time Ensure FLUENT is running in Parallel configuration during launching this utilises multiple computer processors and enables faster solution. As before reduce the element density in the mesh if possible. Reset the relaxation parameters to the default if changing them is not necessary. Reversed flow in _ faces on pressure-inlet/pressure outlet notification This just indicates that the flow direction at a pressure boundary condition varies across its length. The accuracy of the solution will not be effected but computational time is marginally longer. Global courant number is greater than 250. The velocity field is probably diverging error The courant number is a condition which ensures the accuracy of solutions. It is usually a function of the velocity vectors within the domain, and the time step used. An increasing courant number can be rectified by decreasing the time step, but often this is not sufficient. If using variable time stepping, try lowering the minimum step change factor such that the time step can react more sharply to an increasing courant number, or lowering the courant number. In fixed time stepping, simply reducing the time step should reduce the courant number to a level where the velocity field will not diverge Useful Links 1) Learning modules for ANSYS FLUENT mainly uses ANSYS workbench for meshing as opposed to ICEM CFD but the solver (FLUENT) is the same. 2) Explains surface tension & wall adhesion in FLUENT 3) Advises on the use of an appropriate calculation method in FLUENT

21 4) YouTube tutorial for body fitted meshing in a 3D pipe in ICEM CFD. 5) A general guide to modelling multiphase flows in FLUENT 6) Provides numerous potential solutions to a diverging velocity field (Global courant number > 250) 7) Provides potential reasons and solutions for errors encountered when exporting a mesh to FLUENT from ICEM CFD. i ii iii iv