text:
Are you sure?
This action might not be possible to undo. Are you sure you want to continue?
H.S. Pordal, Ph.D. Staff Consultant Stress Engineering Services, Inc. www.stress.com (513) 336 6701 December 8, 2006
Course Summary
This intense course provides a working understanding of Computational Fluid Dynamics (CFD) and an overview of best practices. It is designed to provide the engineer with basic knowledge to apply CFD, identify and solve real life applications. This course creates an awareness of the potentials and limitations of this technology. The engineer will be exposed to a wide range of applications and the course offers high benefits to those who have little or no exposure to CFD. This course offers engineers involved in CFD an opportunity to sample the wide range of applications that can be solved using CFD methods.
Table of Contents
Table of Contents................................................................................................................ ii 1.0 Introduction................................................................................................................... 1 2.0 Overview of CFD.......................................................................................................... 2 2.1 What is CFD ? ........................................................................................................... 2 2.2 Why use CFD ?.......................................................................................................... 2 2.3 Three steps to CFD :.................................................................................................. 3 3.0 Geometry and Mesh Generation ................................................................................... 4 3.1 Flow domain definition : ........................................................................................... 4 3.2 Mesh generation technology:..................................................................................... 6 3.3 Best practices:.......................................................................................................... 10 4.0 Solver Technology ...................................................................................................... 11 4.1 Governing equations :.............................................................................................. 11 4.2 Boundary conditions:............................................................................................... 12 4.3 Discretization:.......................................................................................................... 13 4.4 Linear solvers: ......................................................................................................... 14 4.5 Best practice: ........................................................................................................... 16 5.0 Post Processing ........................................................................................................... 17 5.1 CFD results :............................................................................................................ 17 5.2 Analysis of CFD results: ......................................................................................... 17 6.0 Role of CFD in the Industry........................................................................................ 21 7.0 CFD Applications, Part-I ............................................................................................ 27 7.1 External aerodynamics : .......................................................................................... 27 7.2 Internal flow computations:..................................................................................... 29 7.3 Compressible flow computations: ........................................................................... 31 7.4 Buoyancy driven flows:........................................................................................... 33 7.5 CFD for fluid transport devices:.............................................................................. 35 7.6 Flow in a valve: ....................................................................................................... 40 7.7 Flow and heat transfer: ............................................................................................ 41 8.0 CFD Applications, Part-II........................................................................................... 43 8.1 CFD for mixing applications: .................................................................................. 43 8.2 CFD for multiphase flow:........................................................................................ 45 8.3 Application of CFD to combustion systems:........................................................... 52 9.0 Future of CFD ............................................................................................................. 63 9.1 Limitation of CFD methods :................................................................................... 64 9.2 Next generation CFD:.............................................................................................. 64 11.0 References................................................................................................................ 65
1.0 Introduction
The role of computational methods in engineering design and analysis has greatly increased during the last decade. This is due to improved numerical methods and also due to the advent of faster computers. The computational resources such as computer memory and computer speed are now easily available and also affordable. A desktop personal computer using today's technology can achieve what a super computer achieved about 10 years ago. As a result, the number of engineers applying computational methods for solving engineering problems has also increased dramatically. Mathematical modeling for engineering systems is on the rise. This has lead to a rapid growth in the breadth and depth of software available for analysis. In this course various aspects related to CFD technology are discussed. This course provides the engineer with basic knowledge to identify, apply and solve real life CFD applications. The mechanics of applying CFD depend on the particular software being used. However, the general principles and philosophy described in this course are not specific to a particular software and apply in general.
2.0 Overview of CFD
In this Section a general overview of CFD technology and its merits are discussed. 2.1 What is CFD ? CFD is the process of solving the fluid flow equations of mass, momentum and energy on a computer as applied to a particular geometry and flow conditions. The basic flow variables such as velocity, pressure and temperature are computed at thousands of locations. The CFD solution is based on the first-principle of conservation of mass, momentum and energy. 2.2 Why use CFD ? CFD is a leading edge technology applied to a large number of engineering applications. The benefits of CFD can be summarized as follows: • CFD methods are applied to gain insight into fluid flow and thermal processes. • Complex flow fields for which measurements are not always possible can be analyzed using CFD methods. While measurement probes provide point data, very often full-field data or data at multiple locations is required to fully diagnose a problem. CFD provides data at thousands of locations. • This technology provides a non-intrusive, non-invasive method of fluid flow and heat transfer analysis. • Process scenarios can be examined in a virtual environment, without the safety issues of a real process. For a new design, a number of design concepts can be examined in a virtual environment. • A number of designs can be explored on the computer reducing cut and try methods. Figure 2.2.1 indicates the integration of CFD methods in the design process.
New Product Concept
Process Design
Process & Performance Evaluation
Full Scale Production
Analysis, Trouble-shooting, Rapid Proto-typing CFD Methods
Figure 2.2.1: Role of CFD methods in product design.
2.3 Three steps to CFD : CFD analysis can be broken down into three main steps, viz. Pre-processing, Solution and Post-processing. The main steps of performing a CFD analysis are depicted in Figure 2.3.1.
Analysis of results Extraction of data
Geometry generation
Grid generation
Iterative solution of governing equations
Figure 2.3.1: Steps of performing a CFD analysis Pre-processing: The first step in performing a CFD analysis is called Pre-processing. This involves identification of the flow region of interest, geometric representation of the region, meshing and definition of flow physics. Proper selection of the region of interest and appropriate simplifications play a key role in the success of the calculation. Once the region is defined, a computer model of the geometry is created. The next step is mesh definition. The governing equations are solved at discrete locations in the flow domain. These locations depend on the mesh resolution. The accuracy of a CFD calculation and computer time required for a solution are dependent on mesh resolution. User experience and skill play a crucial role in the choice of a suitable mesh. Once a mesh is created appropriate boundary conditions are applied to define regions of inflow, outflow, walls and other important features. Physical models within the CFD software are activated to simulate flow physics pertaining to the application at hand. For example, a turbulence model is activated to simulate turbulent flow. Selection of appropriate physical models and their applicability to the flow physics at hand is critical to the overall accuracy of a CFD solution. Solution: Once the problem definition is completed it is submitted to the solver for computation of a solution. This step is the Solution step. The governing equations are coupled and non-linear in nature. Therefore a guess-and-correct, iterative strategy is adopted to compute the solution. Post-processing: The third step is Post-processing, during which CFD results are analyzed. A CFD solution provides full-field data; flow variables at thousands, perhaps hundreds of thousands of locations are available. A representation of the flow field is created by plotting flow variables in space on a plane or a line or in a three-dimensional region of interest. The spatial plots give the analyst a 'look inside' the unit which is unavailable experimentally. However, the real value of CFD simulation is frequently found in its ability to provide accurate predictions of integrated quantities such as heat transfer rates, mass transfer rates and forces.
3.0 Geometry and Mesh Generation
In this Section the pre-processing aspect of CFD is discussed. Once the flow region is identified a flow model of the region is created and meshed. 3.1 Flow domain definition : The selection of an appropriate flow domain is key to the success of obtaining a CFD solution. For internal flows, the flow region is defined by the wetted surfaces i.e. surfaces that are in contact with the fluid. Consider flow in a pipe-junction, the flow region is defined by the inner surfaces of the pipes as depicted in Figure 3.1.1 A section upstream and downstream of the pipe-junction is included in the flow domain so that appropriate boundary conditions can be specified. An inflow, outflow and wall boundaries are specified. For external flows, such as flow over an automobile, the flow region includes the region around the automobile. The region ahead, behind and around the automobile is included in the flow domain so that appropriate boundary conditions can be imposed as depicted in Figure 3.1.2. The boundaries at which flow conditions are specified (inflow/outflow) must be far from the region of interest. For this reason the flow domain includes a substantially large region ahead, behind and above the automobile.
Inflow boundary
Wall boundaries
Outflow boundary
Outflow boundary
Figure 3.1.1: Flow region for pipe-junction (internal flow).
Faraway boundaries (flow can leave or enter the computational domain)
Ground Inflow boundary
Figure 3.1.2: Flow region for simulation of flow over an automobile (external flow). While defining the flow domain appropriate simplifications of the flow geometry are required. Features that do not affect the flow behavior in an appreciable manner or are too small to be resolved are not included in the flow domain geometry. As an example, consider modeling the overall flow behavior in the room in which you are currently sitting. The flow domain in this case is enclosed by the walls, floor and ceiling of the room. Objects in the room such as tables and chairs can be represented as rectangular obstacles. The exact shape of the chairs and tables is not modeled to study the overall flow behavior in the room. Objects on the table such as a book, a pen, etc. are not included in the flow model; unless you are specifically interested in the flow around these objects. These objects are too small to alter the overall flow in any appreciable manner. If the thickness of an object is much smaller than the grid size that will be used then the object can be represented as a thin surface (impermeable surface of zero thickness). For instance, the thickness of the chair seat can be ignored and the seat can be modeled as an impermeable thin object with zero thickness. The inflow and outflow regions in the room are the supply and return vents. Engineering judgement along with some understanding of the expected flow behavior is applied in selecting objects that need to be included in the flow model.
Once the flow domain is selected a model of the flow geometry is created. Most commercial CFD packages include a CAD like geometry generation engine. Many CFD packages facilitate easy import of geometry CAD files created by solid modeling packages. A CAD file created for some other purpose such as manufacturing requires modification and cannot be used 'as is' for CFD modeling. CAD created for manufacturing represents the solid region of an object and the flow region is not included in the CAD. For example, CAD created for manufacturing a pipe represents the outer and inner surfaces of the pipe i.e. the solid material of the pipe. Whereas, the flow domain is the region inside the pipe. In such cases, the flow domain is created using the information supplied in the CAD file. 3.2 Mesh generation technology: Once a model of the flow geometry is created it is then meshed. The mesh defines the locations at which the flow solution is computed. The common type of mesh elements used in CFD solvers are hexahedral, tetrahedral, pyramidal or wedge shaped as depicted in Figure 3.2.1. A mesh consisting of hexahedral elements arranged in a rectangular region as depicted in Figure 3.2.2 is known as a single-block structured mesh. A grid cell in a structured mesh can be identified by a unique three-dimensional index (i,j,k). A number of structured blocks can be arranged to define a complex three-dimensional mesh region; such an arrangement is called a multi-block structured mesh. The grid cell in each block is identified by a unique three-dimensional index (i,j,k). Figure 3.2.3 depicts a multi-block structured mesh.
Hexahedral element 8 corners, 12 edges and 6 faces
Pyramidal/wedge element 5 corners, 8 edges and 5 faces Tetrahedral element 4 corners, 6 edges and 4 faces
Figure 3.2.1: Mesh element types for CFD analysis.
J Cell I=3, J=3, K=1 I
Figure 3.2.2: Single-block structured mesh.
Four blocks
Figure 3.2.3: Multi-block structured mesh. Tetrahedral meshing technology allows relatively easy meshing of complex geometries. A surface mesh consisting of triangular elements is first created, this is then used to mesh the inside of the geometry. The grid structure obtained using tetrahedral meshes is called unstructured mesh. Unlike a structured mesh, a grid cell cannot be identified using a single three-dimensional index. A mesh consisting of tetrahedral elements are very
commonly used to mesh complex three-dimensional geometries. For a given mesh length, the number of mesh elements required to mesh a region with tetrahedral elements is about 5-6 times the number of elements required when a hexahedral mesh is created. Very often to optimize the number of elements and for ease of mesh generation, a mixed element mesh consisting of hexahedral elements that transition into pyramids and eventually into tetrahedral elements are used to mesh complex flow geometries. A typical tetrahedral mesh is depicted in Figure 3.2.4.
Figure 3.2.4: Tetrahederal mesh.
The mesh quality has a strong influence on the accuracy of the solution. A poor quality mesh will not only affect the numerical accuracy but also convergence. Mesh aspect ratio and skewness are two parameters that influence mesh quality. Figure 3.2.5 depicts mesh elements with high aspect ratio (width to height ratio). Figure 3.2.6 depicts skewed mesh elements. Rapid changes in mesh density can introduce numerical errors. Mesh size variations must be gradual as depicted in Figure 3.2.7.
Width to height ratio of cells is large
Figure 3.2.5: High aspect ratio mesh elements.
Skewed cells (flat and thin cells)
Rapid change in mesh density
Figure 3.2.6: Skewed mesh elements and rapidly changing mesh density.
Small elements
Gradually varying elements
Large elements
Figure 3.2.7: Gradual mesh size variation.
3.3 Best practices: The type, quality and distribution of mesh elements have a strong influence on the solution. Guidelines for a quality mesh are as follows: • • • • • Select a mesh length that is appropriate for the resolution desired. Avoid large skewness. Aspect ratio of 10 or higher is not normally desirable. Rapid changes in mesh density can have an adverse effect on convergence and accuracy. A change in mesh size between adjacent cells must be less than 2.0.
Some CFD software packages are more forgiving and tolerant of the mesh quality and converge without too much difficult. The actual degree of grid skewness, grid quality, aspect ratio that can be tolerated depends on the flow solver and the flow physics of interest.
4.0 Solver Technology
4.1 Governing equations : The governing equations are conservation equations of mass, momentum and energy. Computational fluid dynamics (CFD) methods are based on first principles of mass, momentum and energy conservation as described by the following equations: Mass:
∂ρ ∂ρu j + = Sm ∂t ∂x j ∂ρui ∂ρui u j ∂P ∂τ ij + + = + Sfi ∂t ∂x j ∂xi ∂x j
∂ρH ∂ρu j H ∂q j ∂uiτ ij ∂p + + + = + Sh ∂t ∂t ∂t ∂x j ∂x j
Where ρ is fluid density, t is time, x is coordinate, u is velocity, P is fluid pressure, H is fluid enthalpy, τ is shear stress and i, j, k = 1,2,3 represent three coordinate directions. Sm is mass source due to reactions or other mass transfer mechanisms. Sf represents momentum source due to mass transfer, body forces such as gravitational force etc. Sh is energy source due to mass transfer, phase change and energy generation by other mechanisms. For situations involving additional species, a conservation equation for each specie is also solved. The transport equation for specie concentration φ is described using equation (4.1.4). ∂ρφ ∂ρφu j + = Ss (4.1.4) Specie: ∂t ∂x j The conservation equations represent rate of change with time, convection into volume and sources. For example, the first term in the mass conservation equation represents rate of change of mass with time, the second term represents the net mass flux. The term on the right-hand-side represents mass source. The source may be due to chemical reactions or any other mechanism by which mass is created. Turbulence modeling Turbulent flow is characterized by rapid fluctuations of flow variables about a mean value. The magnitude of the fluctuations is a fraction of the mean value. Resolving the fluctuations spatially and temporally is quite difficult and not practical in most cases. The effect of turbulent fluctuations is simulated using turbulence models. This involves the solution of additional equations. A number of approaches are adopted to simulate turbulent flow behavior. The approaches vary from simplistic algebraic models for turbulence to complex methods where the fluctuations associated with the turbulent field are captured.
A common approach is to solve Reynolds Averaged Navier Stokes equations (RANS). In this method, the Navier Stokes equations are averaged and the effect of turbulence is represented by using an effective viscosity. Additional equations as defined by the selected turbulence model are solved to compute turbulence related quantities. For example, the k-epsilon turbulence model solves an equation for the turbulent kinetic energy defined by the quantity k and another equation for epsilon the turbulence dissipation rate. A number of turbulence models have been developed. However, the k-epsilon model is applicable to most industrial CFD applications. Flows with swirl or large regions of separation cannot be accurately modeled with k-epsilon model. Variants of k-epsilon model such as RNG or the k-omega model provide an improved solution for such situations. In some cases, more advanced turbulence models such as Large Eddy Simulation (LES) are also applied. In this approach, the large scale turbulent eddies are computed by solving time dependent Navier-Stokes equations. The smaller eddies are modeled using a subgrid model. The large scale eddies are dependent on the flow behavior and geometry; whereas, the small scale eddies are independent of the large scale eddies and can be represented using a subgrid model. LES simulations require a very fine grid so that the large scale eddies can be resolved. A time dependent solution is required so that the unsteady behavior of the eddies is accurately captured. The grid requirements and time step requirements for LES simulations results in large computer resources. LES simulations cannot be easily applied for industrial applications. The most sophisticated level of turbulent flow computations use Direct Numerical Simulations (DNS). In this approach, the time dependent Navier-Stokes equations are solved such that the fluctuations associated with turbulence are captured. This method requires an extremely fine grid and very fine time steps and is not practical for general CFD application. RANS methods provide a viable solution to most CFD applications.
4.2 Boundary conditions: The governing equations are selected based on a problem definition. For example, the energy equation is not selected and solved for isothermal flows. The governing equations are solved subject to boundary conditions. The common surface boundary condition types are velocity specified, pressure specified, outflow or wall. Velocity, pressure and outflow specified boundaries are used to model regions through which the flow can either enter or leave the flow model geometry. At a velocity boundary, the velocity components are specified and this type of boundary is used define the inflow into a CFD model. Pressure boundaries are used to define openings in the flow model through which the flow can either leave or enter the flow domain. An outflow boundary is used to represent regions through which the flow leaves the flow model. Wall boundary conditions are used to represent solid surfaces of the
flow model. A no-slip boundary condition for the velocity is used at walls. For heat transfer applications temperature or heat flux is specified at wall boundaries.
4.3 Discretization: The governing equations are solved using numerical methods. The Navier-Stokes equations are discretized using either Finite Element Methods (FEM), Finite Volume Methods (FVM) or Finite Difference Methods (FDM). Each discretization method has its own advantages and disadvantages.
Finite Difference Method (FDM) is the oldest method for discretization of the governing equations. In this method, the differential form of the equations is discretized using a Taylor series expansion. This is best illustrated using a simple example as described below. A first derivate can be expressed as follows:
dφ/dx = (φi+1 – φi-1)/ 2dx, (4.3.1)
where φi+1 and φi-1 are the values of the variable at the i+1 and i-1 grid points, the grid spacing is dx. The accuracy of the discretization scheme depends on the truncation error which is estimated using Taylor series expansion.
φi+1 = φi + (dφ/dx)i dx + (d2φ/dx2)(dx)2,
Similarly, φi-1 is expressed as a Taylor series expansion about φi using equation (4.3.3).
φi-1 = φi - (dφ/dx)i dx + (d2φ/dx2)(dx)2,
Using equation (4.3.2) and equation (4.3.3) the truncation error associated with the differencing scheme described in equation (4.3.1) is estimated to be of order (dx)2. The differencing scheme in equation (4.3.1) uses the values of the variable on either side of the point in consideration. In other words, the derivative at point i uses the values at points i+1 and i-1. This scheme is known as central differencing and for a first derivative it is second order accurate i.e. the truncation error is of order (dx)2. A differencing scheme that uses the value of the variable only from one-side as illustrated in equation (4.3.4) is called upwind differencing. Using a Taylor series expansion it can be shown that the truncation error is of order (dx). This is scheme provides first order accuracy. (dφ/dx)i = (φi – φi-1)/ dx (4.3.4)
The increased accuracy associated with a second order scheme as compared to that of a first order scheme comes at the price of robustness. At times a second order scheme can create local oscillations in the solution and this can result in a solution process that is difficult to converge or unphysical in nature. The first order scheme is more robust, but provides lower accuracy and tends to smear out gradients. For example, a first order scheme if used to resolve a shock-wave can smear the shock-wave and result in an inaccurate prediction. On the other hand, a second-order scheme can cause wiggles in the
solution around the shock-wave and result in an unphysical situation. To circumvent this difficulty hybrid differencing schemes have been developed. These provide second order accuracy in most regions but reduce to a lower order scheme to prevent unphysical oscillations in the solution. Some such schemes are MUSCL scheme and flux-limited Van Leer scheme.
Finite Volume Method (FVM) uses a control volume approach. The governing equations are integrated over a control volume resulting in a discretized form of the equations. For example, the integration of continuity equation over the control volume depicted in Figure 4.3.1 results in the following form of discretized equation.
(ρ.u.A)w – (ρ.u.A)e + (ρ.v.A)s – (ρ.v.A)n = 0.0, (4.3.5)
The fluxes on the faces are computed using the velocity and density of the neighboring cells. For upwind differencing, the fluxes are computed using the upstream values of the variables. The Navier-Stokes equations are conducive to finite volume discretization and this method can be applied to any general cell type (hexahedral, tetrahedral, pyramidal, etc.). The finite volume method is used in most commercial CFD packages for discretization of the equations.
n u w s v e
Figure 4.3.1: Descretization over a cell.
Finite Element Method (FEM) uses shape functions associated with the element (cell) type for discretization. Weight functions that minimize the error or variation of variable over the element are applied. The Navier-Stokes equations do not naturally lend itself to this method of discretization. FEM is not commonly used for CFD calculations, though there are commercially available CFD packages based on this method.
Some commercially available CFD packages use a hybrid method that uses the key features of FVM along with FEM.
4.4 Linear solvers: The discretized equations result in a non-linear and coupled set of algebraic equations. These are linearized and solved by inverting a matrix. The discretized and linearized equations in matrix form are represented by equation (4.4.1).
where [X] is the solution vector of flow variables (u,v,w,P,T), [A] is the coefficient matrix and depends on the solution vector [X], [R] is the right-hand-side of the discretized equations. The solution vector [X] is obtained by inverting the matrix [A]. Once the solution vector is obtained the matrix [A] is updated and the solution vector recomputed. This process is repeated till equation (4.4.1) is satisfied to a specified degree. The degree to which the solution is satisfied is measured by the residual as defined by equation (4.4.2). [r] = [R]- [A] [X] (4.4.2)
The coefficient matrix [A] is large and cannot be easily inverted using conventional methods of linear algebra. The coefficients of the matrix [A] also depend on the solution vector [X], so an exact inverse is not necessary. The structure of matrix [A] is exploited in computing the inverse. It is very often decomposed into a lower tri-diagonal and upper-tridiagonal matrix also known as LU decomposition. The approximate inverse of matrix [A] is computed by inverting [L] and [U].
[A] = [L] [U] + [E], where [E] represents the error. [X] = [L]-1[U]-1[R] –[E][X]
This results in an iterative process of computing the matrix inverse. The iterations associated with computing the inverse of the matrix are very often referred to as inner iterations and the iterations associated with the non-linearity and coupling between the equations are known as outer iterations. The linearized system of equations is solved using various methods of inverting the matrix [A]. Conjugate gradient methods, algebraic multigrid methods are some such methods. In most commercial CFD software the matrix inversion process is generally transparent to the user. However, the user has control over the outer iterations and this is specified as one of the inputs. The governing equations are non-linear and coupled. A large matrix relating all the variables and equations can be created for the entire mesh. The inversion of this matrix results in a coupled scheme of solution. This is called coupled direct solution method. The matrix is too large and complex to be solved directly. Very often, each equation is solved sequentially resulting in a segregated solution procedure. A matrix is setup for each equation and that equation is solved before proceeding to the next. The size of the matrix in this case is smaller as compared to that for a coupled system. Segregated solution method is adopted in most commercial CFD packages.
The Navier-Stokes equations are coupled non-linear equations and the final solution is obtained using a guess-and-correct solution method. Very often, the initial guess is far from the final solution, the guess-and-correct procedure can lead to divergence of the solution. This is overcome by under-relaxing the solution. The variables are allowed to change gradually using an under-relaxation factor as described by equation (4.4.5).
Φ = ω*Φ1 + (1-ω)*Φ2,
where ω is under-relaxation factor, Φ1 is most recently computed solution and Φ2 is solution at the previous iteration. The typical under-relaxation factor varies between 0.3 and 1.0. A smaller under-relaxation factor is used for more complex cases where the non-linearities are strong. Convergence is assessed by examining the residuals of the equations. The residual represents the degree to which an equation is satisfied. Mass flow balance in the flow domain is often used as the convergence criteria. For incompressible, steady, internal flow the inflow mass flux must match the outflow mass flux within a specified tolerance. A tolerance of less than 1% is typically used.
4.5 Best practice:
• • •
Ensure that the boundary conditions are realistic and represent the flow behavior under investigation. Check that the appropriate flow models have been selected. For example, for turbulent flow ensure that a turbulence model has been selected. Run the flow solver for few iterations, about 10 to 20 iterations and check the boundary conditions. Verify that the flow rate specified at the boundary condition is correct and the direction of flow is correct. Obtain a solution using first-order accurate differencing scheme. If necessary, use this as the starting point for a solution using a second-order differencing scheme. For solutions that are difficult to obtain or if the solution diverges reduce the under-relaxation factors.
• •
5.0 Post Processing
This is the final step of performing a CFD analysis. In this step, the results are extracted and intepretted. 5.1 CFD results : A CFD solution provides full-field data; flow variables at thousands, perhaps hundreds of thousands of locations are available. The velocity components, pressure, density, temperature and other flow related quantities are available from a CFD solution. These quantities are available at the mesh locations used for computing the flow field. The real value of a CFD simulation is frequently found in its ability to provide accurate predictions of integrated quantities such as heat transfer rates, mass transfer rates and forces. The merits of CFD simulation are realized when the relevant information is extracted from the simulation results. This to a large degree depends on the ability and experience of the practitioner.
5.2 Analysis of CFD results: A representation of the flow field is created by plotting flow variables in space on a plane or a line or over a three-dimensional region of interest. The spatial plots give the analyst a 'look inside' the unit which is generally difficult to obtain. The flow behavior can be analyzed by plotting the velocity vectors on a selected plane. Plotting the velocity field over a three-dimensional region can obscure the flow field and is difficult to view. Flow behavior is analyzed by examining the velocity vectors on a series of planes as depicted in Figure 5.2.1a and Figure 5.2.1b. The velocity vector arrows indicate the direction of the flow and the color indicates speed. Regions of flow recirculation can be identified by plotting the velocity field. The vectors can be colored with any other quantity such as temperature. The flow field is also analyzed by examining contours of quantities of interest such as speed, pressure, temperature, shear stress. Figure 5.2.2a depicts the pressure distribution; regions of low and high pressure are identified. Figure 5.2.2b depicts the shear stress distribution on the surface of the automobile. Regions of high shear stress indicate areas of high frictional drag. Line plots to depict the flow behavior or a region of interest can also be created. Figure 5.2.3 shows the variation of speed along the centerline of a pipe. The value of a flow variable at a specific location (point in space) can also be extracted by probing the CFD solution.
Plane 1
Plane 2
Velocity vectors on planes Velocity vectors are colored with speed (m/s)
Figure 5.2.1a: Velocity vectors depicting a flow field in T-junction.
Wake behind automobile
Velocity vectors on mid plane Velocity vectors are colored with speed (m/s)
Figure 5.2.1b: Velocity vectors depicting flow around automobile.
High pressure due to impingement of flow
Figure 5.2.2a: Contours of pressure (Pa).
Figure 5.2.2b: Contours of shear stress (Pa).
Peak pressure due to impingement of flow
Location of line in pipe
Figure 5.2.3: Variation of speed along the center-line of a pipe. Integrated quantities such as drag, lift or components of force can be obtained. CFD is used to compute the lift and drag over airfoils and wings. In many cases the CFD solution is used to compute the forces acting on a body immersed in a fluid. For example, the structural design of turning vanes in a ductwork depends on the flow induced forces on the vanes. In such a case, the forces are estimated using a CFD solution. Surface averaged mean pressure or temperature can also be computed. Mean heat transfer coefficient over a surface of interest can also be computed from a CFD solution. Mean quantities over a volume can also be computed. The mean volumetric concentration of a specie in a region of interest can be estimated from a CFD solution. A CFD solution provides a deluge of information. The flow behavior is analyzed by examining the flow field on planes and lines. Average quantities derived from the flow field are also computed to analyze the flow behavior.
6.0 Role of CFD in the Industry
CFD methods are widely applied within various industries to examine fluid flow and heat transfer behavior. In the Aerospace industry, CFD is routinely applied for aerodynamic calculations, such as computation of lift and drag of lifting surfaces. In the automotive and heavy equipment industries, CFD is applied for external drag calculations, climate control and under-hood cooling. The heating and ventilation industry, power generation industry and chemical process industries, including oil and gas companies, chemical companies, pulp and paper companies and pharmaceutical companies are now beginning to apply CFD methods to gain insight into their various processes. The Aerospace industry has been applying CFD methods for the longest period of time. CFD methods in this industry are routinely applied to improve lift and drag of aerodynamic surfaces. The overall behavior of flow is very well understood and small improvements (on the order of 1%) are sought to achieve incremental increases in performance. In general, CFD methods are applied to understand the overall flow behavior. A typical CFD study is aimed at comparing different designs. 'What-if' studies are performed to examine the influence of various parameters on flow behavior and hence performance. Relative comparison of various designs is carried out using CFD methods. A number of conceptual design changes can be examined rapidly in a "virtual laboratory," without actually building a physical model. CFD study of a full-scale model can be carried out, thus eliminating scale-up issues. Unlike experimental methods, CFD provides full-field data. Pressure, velocity, density, temperature and other quantities of interest are obtained at each and every point in the simulated flow domain. These benefits make CFD a viable tool for analysis, design and rapid proto-typing. CFD technology is now an accepted method of obtaining solutions to fluid flow and heat transfer problems. It has gained a great deal of credibility in many industries and has been integrated into the main stream of design and analysis. In this section, the role of CFD in various industrial sectors is summarized. The typical problems solved using CFD methods are also discussed. Aerospace This industry is engaged in the business of design and fabrication of airborne/space vehicles. It includes major aircraft manufacturers, helicopter, hover craft and space systems generation companies. This industry also includes companies that supply components/units needed by the aerospace companies such as aircraft engines, valves, pumps etc. CFD is widely accepted, applied and regarded as a credible solution method in the Aerospace industry. In fact, CFD was pioneered in the Aerospace industry. 'Homegrown' software is widely applied in this industry and most of the CFD activity is restricted to 'CFD experts'. Applications in this arena include flows over aerodynamic shapes, wings, fuselage, nacelles and after-bodies. CFD is widely applied for analysis of
aircraft components/units such as compressors, pumps, turbines, cross-over elements, nozzles, diffusers and combustion chambers. CFD also plays a role in heat transfer analysis of space systems. These systems typically involve complex flow physics such as radiative heat transfer, micro-convection, multiphase flows and microgravity effects. Leading-edge applications in this industry include full aircraft performance simulations and full engine performance simulations. CFD technology is highly regarded and well integrated into the design process in the aerospace industry. The initial hurdle of 'acceptance' does not exist in this industry. In many cases CFD is the only solution to a problem; for example, design of re-entry and high Mach number systems.
Automotive Major automobile manufacturing companies and those that supply parts, components and design/analysis services for the automobile companies are included in this industrial sector. Design time scales in the automotive industry are very tight; as a result, CFD and FEA analysis techniques are widely used to obtain quick solutions to problems and to evaluate design changes. A typical analyst in this industry is required to perform CFD analysis along with FEA analysis. CFD activity is not restricted to 'CFD experts' only. Typical applications involve flows inside passenger compartments of automobiles, external flows, design of blowers, duct work and under-hood flows. Flow problems related to under-hood cooling are complex and difficult. CFD is also applied for analysis of catalytic convertors, torque convertors, valve design and heat exchanger analysis. Limited application work is carried out for analysis of IC engines. Leading edge applications in this industry include under-hood flow/heat transfer and simulation of combustion in IC engines.
Chemical Process Industry (CPI) Any industry that is involved in the business of processing raw materials for the production of chemicals is classified as CPI. Chemical process industry can be further classified into various sub-industrial sectors as follows: Oil & Gas Chemicals Plastics and Fibers Consumer and health-care products Pharmaceuticals Food Water Metals Mining Fertilizers
Paper and Pulp Glass manufacturers The chemical process industry is quite vast and can be divided into various sub-sectors as outlined in the section above. Some of the larger CP companies have embraced CFD as a viable technology and derived tremendous benefits through its application. These companies have a core group of CFD experts engaged in CFD activity on a full-time basis (similar to the Aerospace industry; however, work is carried out using commercial CFD software). The chemical process industry involves a wide variety of process equipment and a process unit is required to perform a wide variety of duties. Hence, it becomes essential to predict its performance under a wide variety of operating conditions. The flow field involved is very complex and conventional methods of analysis are not adequate. Computational fluid dynamics provides a viable tool for analysis and trouble shooting of such equipment. A typical unit operation processes a large amount of fluid. Given the economics of most unit operations, even small improvements in efficiency and performance can result in a significant increase in revenue and savings in costs. As the process industries enter the 21st century they face new challenges. The predominant forces of change include increased globalization of markets, demands for cleaner environment, higher customer expectations and increased profitability. There has been a general thrust to reduce waste and improve efficiency of processes in general. The traditional approach of taking a product from laboratory scale to pilot plants and then to production is no longer attractive. Process and product development are often initiated simultaneously, as a result, rapid prototyping and analysis is required. To meet these challenges innovation is required at all phases of product development. To meet these goals, Technology Vision 2020, a document highlighting plans for the chemical process industries for the next 20 years has identified three enabling technologies. Computational fluid dynamics (CFD) is one such technology that is expected to lead process companies into the future. The integration of CFD methods will lead to shortened product-process development cycles, optimization of existing processes, reduced energy requirements and efficient design of new products and processes. Unit operations in the hydrocarbon process industry handle large amounts of fluid, as a result, small increments in efficiency lead to large increments in product cost savings. It is thus essential for not only the research and development staff in the hydrocarbon process industry but also for plant managers and production managers to understand the benefits of CFD so that it can be integrated into the development process. Applications in the CPI are very complex and cannot be tackled using an out-of-the-box CFD approach. Judicious simplification and careful examination of the solution process is required. A CFD solution is very often augmented by additional calculations and engineering judgement. Typical applications in this arena involve flows in mixing devices, stirred tank reactors, filtration/separation devices, furnaces, dryers and other equipment. The flow fields are in general very complex, involve multiple phases, mass transfer, heat transfer and very often
reactions. Careful simplification of the flow physics and multi-step solution process is required. The industrial sub-sectors as stated above differ in their core products and processes but the equipment (unit operation devices) applied is similar. Companies are in the process of diversifying their products, as a result, the same process equipment is called on to perform various tasks. Table 6-I summarizes the wide variety of process equipment in the chemical process industry that can benefit from CFD analysis.
Process Equipment
• • Stirred tank reactors, static mixers, jet • mixers, emulsification units.
Impact of CFD
Examine performance of static mixers. Optimize stirred tank performance. Predict shear distribution in stirred tank reactor. Scale-up/scale-down of reactors Establish envelope of performance. Ensure uniform flow distribution. Minimize power requirements. Identify and eliminate sources of erosion in transport of slurry. Optimize and predict performance. Take a 'look-inside' the process. Evaluate design concepts. Minimize failure of heat-exchangers. Control formation of pollutants. Eliminate hot-spots in heaters. Improve flame stability and burner efficiency. Improved heat-recovery. Improved catalyst utilization. Minimize waste. Reduced operating costs. Eliminate plugging, sloshing, spilling.
• Fluid Transport devices: • • Pumps, compressors, manifolds, • headers, valves, flow distributors. • • • Cyclones, scrubbers, precipitators, • centrifuges, gravity separators,
Separation units:
• • Heat exchangers, boilers, furnaces, • process heaters, burners. •
Heat generation and heat transfer:
• • • Packed bed, bubble column, fluidized • bed.
Reactors: Auxiliary processes: Filling, packing.
Table 6-I: Impact of CFD on various processes in the chemical process industries.
To meet the challenges associated with the operation of a wide variety of process equipment, suitable analysis tools are required. The flow fields involved in the chemical process equipment are very complex and conventional methods of analysis are not adequate. Experimental measurement is not always possible. While measurement probes provide point data, very often full-field data or data at multiple locations is required to fully diagnose a problem. Trouble shooting as well as improvements in efficiency and performance are typically achieved by trial and error based on past experience. Failure of a process equipment can result in undesirable downtime and loss of revenue. Hence, more adequate techniques of trouble shooting are required so that downtime can be minimized. CFD has been accepted as a viable tool for the analysis of process equipment.
Electronics Electronic device manufacturing companies such as printer manufacturers, computer hardware manufacturers, silicon wafers suppliers fall under this category. Manufacturing and polishing of silicon wafers is an important process for the electronics industry. CFD has been applied for this process. Chemical vapor deposition is another area of great interest to the electronics industry. CFD is also applied for analysis of micro-electronic devices involving fluid flow and heat transfer such as ink jet printer nozzles. Electroforming, electroplating are some of the other processes analyzed using CFD.
Power Generation Traditionally this industrial sector refers to those industries engaged in the business of generating thermal and hydro electricity. Fuel cells are also part of this industrial segment. This industry can be divided into two main sub-sectors viz. thermal power generation industries and water (hydro) power generation industries. Thermal power generation is normally achieved by combustion of coal in furnaces, energy generated in the furnace is used to produce steam for turbines which are coupled to electric generators. CFD has been applied for analysis of furnaces, burners, duct-work, electrostatic precipitators, coal mills and particle classifiers. The main emphasis here is increased efficiency and lower levels of pollutants. This thrust has given rise to enhanced combustion models and pollutant prediction models in commercial CFD software. The flow physics associated with applications in the power generation industry is quite complex. Hydro-power generation involves generation of electricity from water. CFD has been applied for analysis of water turbines, diffusers, inlet vanes and other auxiliary devices associated with these units.
Fuel cells as an energy source is an emerging technology. The flow physics involved is very complex and CFD is accepted as a technology that can provide insight into design configurations and optimization. CFD software has the capability to analyze the complex physics associated with this technology.
7.0 CFD Applications, Part-I
7.1 External aerodynamics : The flow over an airfoil is computed, the boundary conditions are depicted in Figure 7.1.1. A boundary layer mesh depicted in Figure 7.1.2 is required to accurately compute the flow solution. The velocity and pressure distribution are depicted in Figure 7.1.3 and Figure 7.1.4.
Far field boundary (pressure specified)
Inflow (velocity specified) Outflow (pressure specified) Surface of airfoil (specified as a solid wall)
Far field boundary (pressure specified)
Figure 7.1.1: Flow over an airfoil, boundary conditions.
Fine mesh near surface
Gradually expanding surface mesh
Figure 7.1.2: Mesh near surface of airfoil.
Higher velocity on upper surface
Lower velocity on lower surface
Figure 7.1.3: Velocity (m/s) distribution.
Suction (low pressure) on upper surface
Figure 7.1.4: Pressure (Pa) distribution.
7.2 Internal flow computations: The mixing of two streams in a T-junction is studied using CFD methods. The basic arrangement is depicted in Figure 7.2.1. The mixing is studied by examining the concentration of the side-stream. As depicted in Figure 7.2.2 the fluid from the sidestream lies towards the lower section of the main pipe indicating poor mixing. The mixing behavior is improved by placing a mixing element in the T-junction as depicted in Figure 7.2.3. The concentration of the side-stream for the configuration with a mixing element is depicted in Figure 7.2.4.
Side-stream fluid injection
Main stream fluid
Mixing zone
Figure 7.2.1: T-junction.
Red color denotes 100% concentration of side stream fluid Blue color denotes 100% concentration of main stream fluid
Figure 7.2.2: Mixing behavior in a T-junction.
Mixing element
Figure 7.2.3: T-junction with mixing element.
Dispersion of side-stream due to mixing element resulting in improved mixing
Red color denotes 100% concentration of side stream fluid Blue color denotes 100% concentration of main stream fluid
Figure 7.2.4: Concentration of side-stream fluid in T-junction with a mixing element.
7.3 Compressible flow computations: The compressible flow of a gas in a converging-diverging nozzle depicted in Figure 7.3.1 is computed. Higher order differencing schemes are applied to capture the discontinuities such as shock-wave in the flow. The total supply pressure at the inlet and the static pressure at the outlet are specified. The velocity distribution is depicted in Figure 7.3.2. The Mach number distribution shows acceleration to sonic velocity at the throat. The flow continues to accelerate to supersonic conditions in the diverging portion of the nozzle and decelerates to subsonic conditions through a shock-wave. The location of the sonic regions and the shock wave are depicted in Figure 7.3.4. The pressure distribution is depicted in Figure 7.3.5.
Inflow (Total pressure specified)
Outflow (Static pressure specified)
Figure 7.3.1: Compressible flow in a converging-diverging nozzle.
High velocity region
Figure 7.3.2: Velocity (m/s)distribution in the nozzle.
Sonic region at throat
Supersonic region (ahead of shock wave) Subsonic region (behind shock wave)
Figure 7.3.3: Mach number distribution in the nozzle.
Sonic line at shock wave Sonic region at throat
Figure 7.3.4: Location of sonic regions in the nozzle.
Low pressure due to supersonic expansion in the diverging portion High pressure region behind shock wave
Figure 7.3.5: Pressure (Pa) distribution in the nozzle.
7.4 Buoyancy driven flows: The natural convection currents around a heated pin are simulated. The surface of the pin depicted in Figure 7.4.1 is maintained at a higher temperature than the surrounding air. Buoyancy driven flows are normally unstable and exhibit unsteady behavior. In this case, the plume of hot air rising from the pin sways from one-side to the other as depicted in Figure 7.4.2. The temperature distribution is depicted in Figure 7.4.3.
Open top
Side wall Side wall
Heated pin Bottom wall Bottom wall
Figure 7.4.1: Natural convection around a heated pin.
Region of high velocity in the center of the plume
Swaying of the plume from side-to-side is observed Red color denotes a speed of .74 m/s and blue color denotes are region of zero speed.
Figure 7.4.2: Natural convection velocity distribution (m/s) around the pin.
Swaying of the plume from side-to-side is observed (plume orientation at two different time instants)
Figure 7.4.3: Temperature (K) around the pin.
7.5 CFD for fluid transport devices: CFD methods have been applied for analysis and performance prediction of fluid transport devices such as pumps, compressors and fans. Pumps are commonly employed in the process industries for transport of fluids. Increasing demands for greater productivity very often calls for the same pump to handle different fluids. In the following study CFD techniques are employed to predict pump performance under different operating conditions. Typical flow field is depicted in Figures 7.5.1a and 7.5.1b. The accuracy of CFD solution is demonstrated through detailed comparison with experimental data as shown in Figure 7.5.2.
Figure 7.5.1a: Pump, velocity distribution
12.0 Pressure Rise (inches H O) 10.0 8.0 6.0 4.0 2.0 0.0 0.0 CFD Results Data
Figure 7.5.1b: Pump, streak lines
Flow Rate (gpm)
Figure 7.5.2: Pump performance curve, comparison of CFD results with experimental. CFD is applied to study the flow behavior in a reciprocating pump; a schematic is depicted in Figure 7.5.3. Design changes to eliminate cavitation are explored. As a first step, flow behavior in the existing design is examined. Cavitation occurs during the suction cycle when the fluid is rapidly drawn into the pump. An analysis representing a snap shot of the flow behavior at the instant when the piston suction velocity is highest is carried out. The velocity field in Figure 7.5.4 depicts the flow behavior in the interior of the pump. The incoming fluid impinges on the wall near the discharge port of the pump.
The suction created by the retreating piston creates a helical flow pattern in the chamber as depicted by stream-lines in Figure 7.5.5. This leads to the generation of strong vortices in the pump chamber. The pressure plot in Figure 7.5.6 depicts the low-pressure regions associated with the vortices; red denotes high pressure areas and blue low pressure. These are the regions where cavitation occurs.
Design changes to alter the flow pattern and hence eliminate cavitation are explored. The inlet port of the pump is altered, a wider inlet port is used. The vortical flow pattern within the pump chamber is eliminated as depicted in Figure 7.5.7 and Figure 7.5.8. The pressure profiles in Figure 7.5.9 indicate that overall pressure within the chamber is well above the cavitation limit. Design changes to alter the flow pattern and eliminate cavitation were carried out in a virtual environment
Reciprocating piston
Pump chamber
Inlet port
Outlet port
Figure 7.5.3: Schematic of pump layout.
Figure 7.5.4: Velocity field existing design.
Helical flow path lines
Figure 7.5.5: Path lines in pump chamber.
Low pressure regions
Figure 7.5.6: Pressure distribution in pump chamber.
Figure 7.5.7: Velocity field in modified design.
Figure 7.5.8: Path lines in pump chamber.
Figure 7.5.9: Pressure distribution in pump chamber. Pneumatic transport of products in the form of a powder or a liquid slurry is very common in the process industry. Granular solids of free-flowing natures may be conveyed through ducts with high velocity streams. Air-conveyed materials include chemicals, plastics, pellets, grains and powders of all kinds. Transfer of catalysts between regenerator and reactor under fluidized conditions is a common pneumatic solids transport process. The performance of pneumatic conveyors is sensitive to several characteristics of the solids such as bulk density and particle size distribution. Pressure drop, power requirements are key indicators of performance. Erosion caused by particle impact is an area of concern. Figures 7.5.10a and 7.5.10b depict particle paths for heavy and light particles in a pneumatic conveyer junction. Heavy particles impact the walls of the junction thereby increasing the risk of erosion.
Figure 7.5.10a: Pneumatic conveying, light particle tracks
Figure 7.5.10b: Pneumatic conveying, heavy particle tracks
7.6 Flow in a valve: CFD methods are applied to study the flow behavior in valves and compute valve performance parameters such as flow coefficient. CFD methods are also employed to derive input information for other solution tools. CFD techniques are employed to obtain pressure distribution and flow characteristics of a butterfly valve at various valve openings. The valve positions and flow behavior are depicted in Figure 7.6.1. The discharge coefficient vs angle computed using the CFD model is applied as input to a waterhammer calculation tool. The resulting waterhammer pressure profile is depicted in Figure 7.6.2.
Pressure @ 0 Degrees
Pressure @ 45 Degrees
1.5 Relative Head at Valve Valve Position
Pressure @ 85 Degrees
Figure 7.6.1: Butterfly valve, pressure distribution for various positions
Relative head at valve
-1 0.2 0 0.2 0.4 0.6 0.8 1
TIME (seconds)
Figure 7.6.2: Butterfly valve, Water-hammer profile
7.7 Flow and heat transfer: CFD for Heat generation and heat transfer equipment: Heat transfer equipment such as heat exchangers are employed throughout a chemical processing plant. Failure of this equipment can lead to downtime and significant loss of revenue. Hence, it is essential for this equipment to perform as reliably as possible. Inefficiencies associated with heat transfer equipment directly influence production cost. Small increments in improved efficiency can result in significant reduction of operating cost and increased revenues. CFD techniques can provide an insight into the function of these devices and can help identify areas for improvement. Figure 7.7.1a shows the temperature distribution over an array of cylinder in cross flow. This is a very common configuration in heat exchangers. Comparison of CFD results with experimental data is depicted in Figure 7.7.1b.
2x2 Tube Bundle Heat Transfer Coefficients
70 Tube 1 HTC - Correlation (Btu/hr/ft^2-F)
Tube 1 HTC - Correlation Tube 1 HTC - CFD Core Tube HTC - Correlation Core Tube HTC - CFD
10 0 20 40 60 80 100 120 Inlet Velocity (ft/s)
Figure 7.7.1a: Heat exchanger, temperature distribution
Figure 7.7.1b: Comparison of CFD results with data
Process heaters of various types are employed for endothermic reactions. The two major types of heaters are direct-fired or indirect-fired. Direct-fired heaters are typically employed for hydrocarbon reforming, pyrolysis-type of processes. High process temperatures are achieved by direct transfer of heat from the products of combustion of fuels. Heat is released by the process of combustion which is transferred to fluids inside tubes which are arranged along the walls and roof of the combustion chamber. Tubes containing the process fluid are subject to combustion process gases and high temperatures. If the heating is not uniform then hot-spots may occur leading to failure; on the other hand, inadequate heating can lead to lower process fluid temperatures and inefficiencies. Formation of pollutants such as NOx can be reduced using design guidance provided by CFD simulations. The combustion process and heat transfer within direct-fired heaters are very complex. Simple methods are inadequate to analyze and predict performance. Experimental
measurements are difficult and even impossible. Computational methods such as CFD present a viable approach for analysis of such equipment. The combustion process and heat transfer in a direct-fired heater are modeled using computational fluid dynamics. A vertical-cylindrical radiant process heater is modeled. The tubes containing the process fluid are arranged helically as a coil along the walls of the combustion chamber. Firing of fuel is vertical from the floor. Heat transfer to the process tube and uniformity of the temperature field are examined and depicted in Figure 7.7.2, red regions denote high temperature and blue regions correspond to low temperature. It is observed that the heat transfer to the tubes is quite uniform. However, the exhaust gas temperature is high, indicating that a heat recovery unit downstream of the primary heater may need to be installed to recover waste heat.
Figure 7.7.2: Process heater, temperature distribution.
8.0 CFD Applications, Part-II
8.1 CFD for mixing applications: Mixing processes form the heart of the chemical process industries. Mixing may involve blending of two streams of the same fluid but at different temperatures (thermal mixing) or, it may involve mixing of two or more different fluids with or without chemical reactions. The degree of mixing required and the equipment applied depends on the actual application. Static mixers for fluid-fluid mixing and stirred tanks are by far the most commonly applied units for mixing. Stirred tank reactors are very commonly used in the chemical process industries for a wide range of duties. The primary function of these vessels is to provide adequate stirring and mixing of a mixture. The mixing characteristics influence the product quality and efficiency of the process to a great degree. Stirred vessels come in various shapes, sizes and are equipped with many different types of impellers. Very often the same vessel is required to perform various duties and it is essential for engineers to ensure that adequate shaft power is available to perform the mixing duty. More importantly, it is essential to ensure efficient operation of the vessel for a given duty. This is very often accomplished by placing the impellers in the vessel at various locations. Empirical correlations for estimating vessel performance exist. However, these correlations are unable to predict the performance accurately and are very often based on the assumption of linear superposition of data. The following study examines the influence of impeller location on the flow field. CFD methods are employed to analyze the flow field and study vessel flow characteristics. Single-phase flow in a flat-bottom, baffled tank with dual 4-bladed Rushton impellers is modeled. Rushton impellers are typically employed to generate radial flow. Figure 8.1.1a shows properly placed impellers in the vessel. The radial flow field generated by the impellers leads to formation of four torroidal re-circulation regions. The impellers in this case operate with little if any interaction between them. If the impellers are placed closer to each other, a converging flow pattern is generated. This is depicted in Figure 8.1.1b. The upper impeller pumps downward and the lower impeller pumps upwards. However, if the impellers are placed further apart, a diverging flow pattern as depicted in Figure 8.1.1c is generated. In this case, the lower impeller pumps downward and the upper impeller continues to pump radially outwards. Changes in impeller position lead to a drastic change in the flow pattern. This has a strong effect on vessel performance, mixing characteristics and hence product quality and efficiency. Impeller-impeller interaction is a strong non-linear effect and cannot be predicted by simple empirical correlations. CFD provides a viable method to analyze and optimize stirred tank performance. Impeller performance and flow field characteristics can be successfully predicted using CFD methods. CFD methods can also be applied to predict shear stress distribution within a stirred vessel. This is important for dissolution, emulsification and dispersion. Shear stress
distribution is also important for biomedical applications where excessive shear may lead to damage of product and loss of efficacy.
Figure 8.1.1a: Stirred tank, radially pumping impellers
Figure 8.1.1b: Stirred tank, closely placed impellers
Figure 8.1.1c: Stirred tank, impellers too far apart
CFD is also applied to study the flow behavior in static mixers. Static mixer design and element shape and size can be optimized using CFD methods. Figure 8.1.2 depicts the mixing of two fluids in a static mixer.
Helical ribbons for mixing
The fluid streams are colored red and blue
Figure 8.1.2: Mixing of fluids in a static mixer.
8.2 CFD for multiphase flow: Flow fields in the chemical process unit operations are complex and often involve multiphase flows. Multi-fluid flow also referred to as multiphase flows are complex in nature and difficult to measure and analyze. A full description of multiphase flow modeling methods is provided in Appendix A. CFD Study of Spray Dryer: Drying equipment is usually large and expensive. As a result, efficiency is an important factor that influences production and operation cost. In this section the benefits derived from CFD study of a spray dryer are discussed. CFD is used to analyze the performance of a tall-form powdered milk industrial spray dryer in advance of making major structural changes to the dryer. The risk of lost profit during changeover (especially if the improvement did not materialize) is minimized. CFD is applied to examine configuration changes and thus minimize risk and avoid unnecessary downtime during testing. CFD results can provide the necessary confidence that the proposed modifications will work before capital equipment is ordered and fieldtesting scheduled. A tall-form powdered milk spray dryer is analyzed. An Eulerian-Lagrangian model is applied to simulate the flow field in the spray dryer. The gas phase is simulated using an Eulerian formulation. The spray drops are simulated using a discrete particle model. In this case, the drops exchange mass, momentum and energy with the continuous phase. Full coupling between the phases is required to produce an accurate simulate. The CFD results are applied to guide changes in the geometry and process parameters necessary to improve product quality. Different combinations of axial and swirling airflows are modeled. Figure 8.2.1 depicts the velocity field in the dryer. The velocity field is skewed towards the wall. This is a result of non-uniform pressure distribution in the air dispersing head. By changing the vane angles of the air disperser along with nozzle spray patterns it is possible to create optimum conditions within the dryer thus yielding a product with desirable qualities and reducing powder buildup on the dryer walls.
Skewed velocity field
Figure 8.2.1: Spray dryer, velocity field CFD Study of Cyclone: In this study CFD solutions are applied to optimize and predict performance of an existing cyclone design. Eulerian-Lagrangian model is applied to simulate the flow field. The gas phase is simulated using an Eulerian formulation. The particles are simulated using a discrete particle model. In this case, the particles exchange momentum with the continuous phase. Momentum coupling between the two phases is included. Separation efficiency for different particle sizes is examined. Figures 8.2.2a and 8.2.2b depict particle paths for various particle sizes. CFD techniques are employed to perform 'what-if' analysis for optimization of the design. The results agree well with tests, showing a marked fall-off in separation efficiency between 1 µ m and 10 µ m size particles.
Figure 8.2.2a: Cyclone, path line of 1micron particle
Figure 8.2.2b: Cyclone, path line of 10 micron particle
CFD Study of Filling: CFD is used to simulate the filling process of containers. A number of 'virtual experiments' are conducted to optimize the filling process. A number of filling profiles are examined to minimize splashing. An Eulerian-Eulerian Volume of Fluid (VOF) model is applied. This study involves free surface tracking so a volume of fluid method is applied to track the free surface. Inertial effects dominate and surface tension force effects are negligible; therefore, a surface tension model is not included. The free surface is tracked at various time instants and filling profile adjusted to eliminate splashing of fluid. Free surface shape and location at the start of filling cycle is depicted in Figure 8.2.3a and Figure 8.2.3b. Red color denotes liquid and blue gas.
Red color denotes liquid and blue air Smooth filling Splashing of liquid on sides
Figure 8.2.3a: Filling process, free surface location. Figure 8.2.3b: Filling process, free surface location. Strong splash. No splash.
CFD Study of Drop Injection: Drop and bubble formation are studied to establish injection characteristics and understand sparger behavior. In this study, an EulerianEulerian homogenous flow model is applied to study drop formation from a nozzle. The inertial forces associated with such flow fields are small and surface tension effects dominate. Shape, size and frequency of drop formation are examined. Liquid is injected through an injection tube, the injected fluid initially collects at the nozzle tip as depicted in Figure 8.2.4a. As the fluid bubble grows in size the gravitational force becomes large and necking of fluid takes place as depicted in Figure 8.2.4b. At this stage, the fluid column is no longer able to hold the ejected fluid in place and it breaks from the nozzle forming a drop as depicted in Figure 8.2.4c.
Figure 8.2.4a: Initial collection of fluid at nozzle tip
Figure 8.2.4b: Necking of injected fluid
Figure 8.2.4c: Drop formation
CFD Study of Centrifuge Separation: Industrial centrifuges are widely used in the process industries for separation of solids from liquids and liquid-liquid separation. If the density of the two fluids is similar, then gravitational separation is no longer effective, centrifuge separation devices can be effectively employed under these conditions. In general, centrifuges are used for thickening, separation and post-treatment. Centrifuge separators are required to provide better separation quality materials at lower operating costs. This is achieved by improvements in existing design as well as developing new ones. In the present study, design modification to a centrifuge shown in Figure 8.2.5a are examined using computational fluid dynamics (CFD). A drift-flux model is applied to simulate the flow field. The solution is computed in a rotating frame of reference. The original design results in slugging of material. This behavior is characterized by the transient flow field observed during the simulations. Figures 8.2.5a and 8.2.5b depict material density at two different time instants. As part of design change investigations, the concentrate outlet port (side port) was closed. This resulted in high density liquid exiting the low density port; this situation is undesirable. Next, the side port opening was reduced. This minimized slugging and a near steady flow field is observed as shown in Figure 8.2.5c. Heavy Fluid Outlet Light fluid outlet
Concentrate outlet
Concentrate outlet
Inlet Figure 8.2.5a: Centrifuge configuration
Figure 8.2.5b: Fluid density (original design) (modified design)
CFD simulation of bubble column reactor: Bubble columns reactors are used for contact operations involving gas and liquid. The flow field within such reactors is very complex. In the present study, gas-liquid flow in an airlift loop reactor is simulated using an Eulerian-Eulerian two phase flow model. The bubbles are modeled as a dispersed phase and the liquid is treated as a continuous phase. Figure 8.2.6 depicts the gas phase distribution and liquid phase velocity field in the reactor. CFD solution is used to predict the bubble distribution in the reactor so that design changes to improve efficacy of the process can be planned.
Figure 8.2.6: Gas flow distribution. (Courtesy of
AEA Technology)
CFD study of gas-solid flow in a fluidized catalytic cracking unit : gas-solid flows are very commonly observed in chemical process industries. Pneumatic transport of solids, catalytic cracking are some examples of such flows. In the petrochemical industries, fluidized bed reactors are employed for catalytic cracking of hydrocarbons. Figure 8.2.7 depicts gas flow progression through a FCC riser. The flow field is simulated using an Eulerian-Eulerian model. The solid phase is treated as a dispersed phase. A solids pressure model is included to account for particle-particle interaction. CFD is applied to study the flow field in devices such as a FCC is unsteady and chaotic. Simulation of such a flow field requires unsteady flow calculations. Small time increments are required to simulate such flow fields, as a result, these calculations can be very time intensive. Simulations of gas-solid flows in complex three-dimensional reactors can take months of computational time and are not practically feasible. However, with the advent of faster computers and parallel processing capability simulation of gas-solid flows in complex reactors can become a reality.
Figure 8.2.7: Gas flow progression in a fluidized bed riser. (Courtesy of
AEA Technology)
Flow fields in the chemical process unit operations are complex and often involve multiphase flows. Analysis of multi-fluid or multiphase handling devices is not easy; conventional methods are inadequate and experimental measurement is difficult if not impossible. Computational Fluid Dynamics (CFD) has been identified as a viable tool for analysis of such devices and associated flow fields.
8.3 Application of CFD to combustion systems: CFD techniques can be applied for design, analysis and troubleshooting of combustion systems. Problems associated with high excess air, high stack temperature, flame impingement, non-uniform temperatures, loss of efficiency and non-uniform flow distribution can be examined. CFD techniques provide an insight into combustion systems such as burners, furnaces, boilers, heaters and reformers. These methods can also be applied for the analysis of auxiliary components such as wind-boxes, classifiers, precipitators and scrubbers. Combustion Modeling Combustion is the process by which heat is rapidly released by oxidation of a fuel. The main products of combustion are carbon dioxide and water vapor. Combustion is a very complex physical process involving strong interactions between the aerodynamic field, thermal field, turbulence interactions, mixing and chemical kinetics. These physical processes are tightly coupled to each other. In many cases, fuel is injected in the form of particles or droplets. In such cases interaction between the gas phase and the particulate phase plays an important role. Combustion models that appropriately account for the above effects have been developed. Combustion systems involve high temperatures. At these temperatures heat transfer by radiation plays an important role. An appropriate radiation model must be included when simulating combustion systems. Computational models that account for thermal, prompt and fuel NOx have been developed. Soot and NOx formation are modeled using semi-empirical mechanisms. These mechanisms are not very reliable and accurate prediction of absolute quantities of pollutants is difficult. However, the models can be applied for relative comparison of designs and also to predict trends.
CFD for Boilers: Boilers are used to convert energy in conventional fuels (coal, oil and gas) to steam for power generation, heating or process consumption. There are two main types of boilers. Fire-tube boilers are those where combustion takes place inside tubes and steam is generated on the outside. These are typically used in small package-boilers and also in waste-heat recovery units that operate at medium or low-pressures. The other types are water-tube boilers; these are more commonly used. In these units, water passing through tubes is heated using combustion gases. These are available in a wide range of capacities, ranging from 5,000 lbs/hr to as high as 9,000,000 lbs/hr of steam. These units typically employ natural gas, oil or pulverized coal as fuel. A water-tube boiler consists of various components such as burners and heater tubes. Burners of various types are employed to inject, mix and burn fuel and oxidant. The combustion process is completed in the furnace section of the boiler; heat is extracted in the radiant and convection section of a furnace. The radiant section of a furnace is lined with water-tubes; steam is generated in this section by radiant heating of the tubes. The convective section consists of tube banks and heating of fluid in the tubes is accomplished by passing hot combustion products through the tube bank. This section is
also referred to as the superheater section and generates high-pressure steam. Many boilers also include an economizer unit. This unit extracts heat from the moderate temperature gases leaving the superheater section. Air heaters are employed to further extract heat form the gas before discharging to stacks. This heat is recycled to the furnace with combustion air. Coal-fired furnaces employ pulverized coal as the fuel. Pulverized coal is mixed with air and burnt in the furnace section of the boiler. Various configurations of coal-fired furnaces exist. In wall-fired furnaces, swirl-type burners are located on one of the vertical walls of the furnace. Swirl imparted by the burner to the secondary stream of air creates a recirculation zone in front of the burner. This region acts as a flame stabilizer and is the primary combustion zone in the furnace. Tangentially-fired or T-fired furnaces are more common. Burners are located on the boiler corners and fire towards the axis of the furnace. This generates a vortex in the core of the furnace; combustion takes place in this region. Coal requiring high residence times and higher temperatures is burnt in down-fired furnaces. In this case the burners are located on horizontal walls in the furnace and fire downwards. Cyclone furnaces differ from the conventional T-fired or wall-fired furnaces. In a cyclone furnace, coal devolatilization and char oxidation occurs in a separate cyclone-type chamber. Residence of coal is increased by generating highly swirling flow in the chamber. This chamber also retains most of the coal ash and slag.
The flow field within boilers is very complex and involves interaction between many variables such as fuel characteristics, firing systems, and heat transfer. CFD methods can be applied to examine and study complex flow behavior. The furnace enclosure is one of the most critical components of a boiler. Uniform gas flow and temperatures are desired in the convective section of the furnace. Nonuniformities can result in hot-spots and excessive metal temperatures in the boiler tubes, resulting in failure. CFD modeling of package gas-fired boiler: A gas-fired boiler as shown in Figure 8.3.1 is analyzed. The burner is shown in Figure 8.3.2 and consists of a fuel lance. The oxidant is introduced through the annular space and passes through a set of swirl-vanes. The swirl imparted by the vanes stabilizes the flame. The temperature plot in Figure 8.3.3 depicts the high temperature region in the convective section of the furnace chamber. This is the region where boiler tubes are most likely to fail. The velocity field in Figure 8.3.4 depicts a low velocity region near the outer surface of the radiant section. However, the temperatures in this region are acceptable. Design changes to induce a more uniform temperature field in the convective section of the furnace can be explored using CFD methods.
Boiler tubes section
Radiant section Figure 8.3.1: Boiler layout.
Swirl vanes
Fuel Lance
Figure 8.3.2: Boiler configuration.
Figure 8.3.3: Temperature distribution in boiler (temperatures in oK).
Figure 8.3.4: Velocity distribution in boiler (velocity in m/sec)
Application of CFD for coal-fired furnace: Coal-fired furnaces are employed by utilities for power generation. Uniform flow and temperatures are desired in the furnace. Minimization of unburned combustible loss in the fly ash from pulverized coal-firing units, slag formation and deposition are other issues that affect the performance of such
devices. NOx formation and unburnt carbon have an environmental impact. These aspects can be examined using CFD methods.
A coal-fired unit as shown in Figure 8.3.5 is analyzed. The burners are arranged at three elevations in the unit. Figure 8.3.6 shows the path of coal particles in the furnace. The results indicate that very few coal particles settle at the bottom and contribute to slag formation; most of the particles are carried away by the flue gas. Figure 8.3.7 depicts the velocity field in the furnace, the swirling motion of the gas helps in flame stabilization and increases heat transfer to the furnace walls. Design changes to improve unit performance and NOx reduction can be explored using CFD methods.
Coal inlets shown in red Secondary air inlets in green.
Figure 8.3.5: Coal-fired furnace.
Figure 8.3.6: Coal particle path-lines in furnace.
Figure 8.3.7: Velocity field in furnace.
CFD for Burner analysis: Flame stability and burner efficiency are very critical to the proper functioning of a process heater, power plant or furnace. Flame length, shape and size can influence the process. If the flame is too long it can impinge on critical regions of the apparatus and cause thermal damage. If it is too short it may wear out the burner
tip. Replacement of the burner or associated apparatus results in downtime and loss of revenue. Computational fluid dynamics modeling methods can be applied to gain insight into flame characteristics. Appropriate burner configurations can be arrived at through CFD. Performance of retrofitted burners for low NOx can be evaluated using CFD before actually installing such a unit. Natural gas burner: In the present study a natural gas burner is modified. The flame length, shape and size are examined for two burner configurations. In this case fuel injection lance modifications are examined to study the effect on flame length, shape and size. The fuel lance tip is modified, results are depicted in Figures 8.3.8 and 8.3.9. Introduction of a disk at the lance tip to inject fuel gas through a conical slot results in a much shorter flame and desirable characteristics. The placement of burners for optimum furnace, boiler or process heater performance can be examined through CFD analysis.
Figure 8.3.8: Fuel lance without tip modification. Fuel gas is injected axially.
Figure 8.3.9: Fuel lance modified , fuel gas injected through an conical slot.
CFD for auxiliary components: A power plant consists of various flow-carrying devices. The performance of a boiler or a furnace is greatly influenced by proper functioning of auxiliary components such as a windbox and the associated ductwork. CFD analysis of flow distribution in ducts: CFD techniques can be applied to achieve proper flow distribution. Figure 8.3.10 depicts the air-flow distribution in a power-plant ductwork. Flow rates through the various branches of the ductwork are computed. Dampers and flow deflectors can be included to introduce even flow distribution.
Figure 8.3.10: Velocity distribution in air-flow ducts in a power-plant (velocity in m/sec). CFD based optimization of an electrostatic precipitator: CFD methods can also be applied to optimize and enhance performance of flow separation devices such as precipitators and scrubbers. Electrostatic precipitators (ESP) are very effective in the removal of fine mists and fine particles from gas streams. Atmospheric dust concentration measurement is also achieved by employing electrostatic precipitators. A typical electrostatic precipitator is comprised of ductwork and a diffuser section. Electrostatically charged filters are located in the diffuser section. Effective performance of an ESP requires uniform flow in the diffuser section. The upstream ductwork can have a significant impact on the flow entering the diffuser and hence its effectiveness and performance. These devices are several meters in size and are difficult to prototype. Expensive experimental setups may be constructed to study the flow fields in such devices. The other option is numerical simulation of such flow fields. This option is relatively inexpensive and can be completed on a smaller time scale. CFD methods are routinely employed to examine ESP performance. In the following study, CFD is applied to examine the effect of various distributor plate configurations on the uniformity of flow entering the diffuser section of an ESP. The original design employs a grid type distributor plate. The flow entering the diffuser is not uniformly distributed and continues as a jet in the core of the diffuser section. This leads to a large recirculation region in the ESP as depicted in Figure 8.3.11. In an attempt to introduce more uniform flow in the diffuser, various splitter plate configurations were examined. A grid employing three vertical and three horizontally placed splitter plates produced the best results. The velocity field is depicted in Figure 8.3.12. CFD methods can be rapidly applied to examine the effect of various geometric and flow parameters on the overall flow behavior in an ESP. These techniques can be applied for troubleshooting, improving the performance and also for rapid prototyping.
Figure 8.3.11: Velocity distribution in original ESP design (velocity in m/sec).
Figure 8.3.12: Velocity field in modified ESP design (velocity in m/sec).
CFD for NOx reduction: Emission control is a key issue for industries engaged in utilization of combustion systems. NOx or oxides of Nitrogen have an adverse effect on the environment. These pollutants lead to the formation of ozone, smog and acid rain. Figure 8.3.13 depicts NOx distribution (ppm) in a gas-fired package boiler. Higher NOx concentration is observed in the fuel rich region. Two major approaches are adopted for NOx reduction. These are pre-combustion control techniques and post-combustion treatment.
Pre-combustion NOx control methods reduce the formation of NOx by modification of combustion conditions. This is achieved by low excess air, staged combustion, temperature reduction, deployment of low NOx burners, oxygas combustion, reburn, flue gas recirculation. The design and conceptual testing of low NOx concepts can be achieved using CFD methods. CFD techniques can be employed to identify the most promising concept and reduce the number of iterations with trial-and-error methods.
Post-combustion NOx reduction methods involve removal of NOx from the flue gas using selective catalytic reduction (SCR) or selective non-catalytic reduction (SNCR). SNCR methods can reduce NOx by about 45%, whereas SCR techniques can reduced NOx by 70%. SCR process consists of injecting ammonia into the boiler flue gas and passing the flue gas through a catalyst bed where NOx reacts with ammonia. SCR reactors are installed between the boiler and air heater; space is limited and the duct work required to distribute flow in the SCR reactor is complex. The design of this can be achieved using CFD methods. CFD methods can be employed to optimize flow distribution within the SCR reactor. Injection and mixing of ammonia in the flue gas can be optimized using CFD methods. A properly designed system can result in reduced ammonia slip. Catalyst utilization in SCR reactors can be maximized to reduce operating costs.
Figure 8.3.13: NOx distribution (parts per million) in a package boiler.
9.0 Future of CFD
Technology Vision 2020 has identified CFD as a key technology that will enable the process industries meet challenges of the future. The integration of CFD methods will lead to shortened product-process development cycles, optimization of existing processes, reduced energy requirements and efficient design of new products and processes. Unit operations in process industries handle large amounts of fluid, as a result, small increments in efficiency lead to large increments in product cost savings, CFD solutions can help accomplish this. The number of processes that can be improved with the aid of CFD techniques are many. Aerospace and automobile industries have already integrated CFD methods into their design process. The process industries are now beginning to accept this technology; however, it is yet to be fully integrated. The potential for process improvements using CFD solutions is yet to be realized. Applicability of CFD techniques for design, analysis and troubleshooting of pumps has been discussed. CFD provides an important new tool to the pump designer. CFD can be used to dramatically reduce the number of iterations required in the typical design cycle. It can be used to trouble-shoot existing designs and evaluate new design concepts in a 'virtual environment'. It is a tool that can provide substantial savings in both time and cost during the pump development cycle. CFD applications to a number of unit operations and processes in the chemical process industries, oil and gas industry. In general CFD methods are applied to understand the overall flow and heat transfer behavior. A typical study is aimed at comparing and evaluating designs or concepts. 'What-if' studies are performed to examine the influence of various parameters on flow behavior and hence performance. Unlike experimental methods, CFD provides full-field data. CFD technology is widely accepted and applied within various industries. Commercial CFD software has matured over the years. A number of commercial CFD software packages are available. CFD solvers are wrapped in a user-friendly graphical interface (GUI). These general-purpose CFD software packages can be applied to simulate fluid flow, heat transfer, chemical species transport and reactions for a wide variety of applications. The look, feel, performance and accuracy may differ from one CFD package to another. However, the basic principles and steps involved in performing a CFD analysis is the same. .
9.1 Limitation of CFD methods : The use of CAD for analysis is still a daunting task. CAD information is readily useable for manufacturing but not for analysis. Commercial CFD software packages claim CAD compatability, which very often means merely the ability to read CAD. Most often CAD supplied for analysis is originally generated for manufacturing and is not suitable for analysis. The supplied CAD requires substantial manipulation before an analysis package can use it. The pre-processors (geometry and mesh generation) supplied with CFD packages are not designed to handle CAD. Meshing techniques in CFD packages require modification so that CAD can be handled in a seamless manner . CAD plays a role when analysis and modification of existing designs is involved. However, CAD data is rarely used during the evaluation of design concepts. The automotive industry is CAD centric to a large degree. CAD data is uncommon in the CPI and power generation industries. In these industries, CFD geometry models are created from existing paper drawings of process equipment. The ability to create, manipulate, modify geometry and mesh with ease is a limitation of this technology.
9.2 Next generation CFD: Commercial CFD software has evolved considerably during the past decade. Geometry generation and mesh generation tools have become more intuitive and user-friendly in nature. Unstructured meshing has been a boon for modeling complex geometry. CFD solvers are more robust and require minimal user intervention. Post-processing capability within CFD software has increased substantially. Models for complex physics have been included in CFD software. These are tremendous enhancements to underlying CFD technology. As a result, the utility of commercial CFD software has increased dramatically. However, these are all enhancements that are confined to the traditional CFD approach and the underlying CFD paradigm. Commercial CFD suppliers define the attributes of the next generation CFD software as having highly parallelized solver, coupled solver, automatic-grid adaption, etc. These are again enhancements within the CFD paradigm. These enhancements are likely to reduce the time required for CFD analysis and expand the use of CFD marginally across to the non-expert user. Specific tools for specific industries are required. These tools would be built on the current, mature, robust and highly evolved CFD technology. Specific knowledge related to these industries would be included in these tools.
11.0 References
1) Department of Energy (DOE). CFD Technology Roadmap, Technology Vision 2020: The U.S. Chemical Industry, 1998. 2) Perry, R.H., Green. D., Chemical engineers' handbook, Mc Graw Hill, 1984. 3) Patankar, S.V., Numerical heat transfer and fluid flow, Hemisphere, 1983. 4) Anderson, D.A., Tannehill, J.C., Pletcher, R.H., Computational fluid mechanics and heat transfer, Mc Graw Hill, 1984. 5) C.J. Matice., T.J. Fry., E.M. Luther., Computer flow modeling for pump performance, Appliance engineer, January 2001. 6) H.S. Pordal., C.J. Matice, T.J. Fry., Computational fluid dynamics: a key analytical tool, Hydrocarbon processing, August 2001. 7) H.S. Pordal., C.J. Matice, T.J. Fry., Using CFD models to simulate multiphase flow, Chemical processing, November 2001. 8) C.J. Matice., High speed filling of plastic containers. SME, November 1997. 9) H.S. Pordal., SES review of liquid-liquid mixing, mixing equipment and ultrasonic emulsification, SES report March 2001. 10) H.S. Pordal., SES review of mixing for scale-up and scale-down, SES report November 2001. 11) T.J. Fry., CFD aids in the development of novel spray drying technology, Powders and bulk magazine, 2001. 12) C.J. Matice., H.S. Pordal., Design of venturi mixers, Flow control magazine, November 2001. 13) Harnby, N., Edwards, M.F., Nienow, A.W., Mixing in the process industries, Butterworth Heinemann, 1992. 14) Tatterson, G.B., Fluid mixing and gas dispersion in agitated tanks, Mc Graw-Hill Inc., 1991. 15) Tatterson, G.B., Scaleup and design of industrial mixing processes, Mc Graw-Hill Inc., 1994. 16) OIT, Industrial combustion technology roadmap, 1999. 17) Turnis, S.R., An introduction to combustion, Mc Graw Hill Series, 1998. 18) Kuo, K.K., Principles of combustion, John Wiley and Sons, 1986. 19) Black, P.O., Pumps, Howard W. Sams and Co, 1970. 20) Matice, C.J., Fry, T.J., Luther, M., Computer flow modeling for pump performance, Appliance engineer magazine, January 2001.
Appendix A Introduction:
A chemical processing plant employs a wide variety of process equipment. Fluid transport equipment, heat generation and heat transfer equipment, drying equipment, mixing and agitation equipment, separation devices, and reactors are some of the unit operations that constitute a chemical processing plant. The flow through these units is very complex. This complexity arises partly due to the geometric complexity of the unit and partly due to the nature of the flow field itself. The flow field is often complicated by the presence of multiple fluids. Multi-fluid flows also referred to as multiphase flows are complex in nature and difficult to measure and analyze. Conventional methods of analysis based on one-dimensional co-relations do not provide an adequate description of the flow field. Scaling methods and dimensional analysis for single-phase flows exist. However, dimensional analysis for multiphase flows is difficult and complex. Scaling requirements are difficult to satisfy across a range of flow patterns. Overall models of systems exist; these depend on large number of correlations, closure and constitutive relations. System models are one-dimensional in nature, system-specific and cannot be applied to general situations. Experimental measurement is not always possible. While measurement probes provide point data, very often full-field data or data at multiple locations is required to fully diagnose a problem. Scale-up and extrapolation issues associated with testing are far more complex for multiphase systems. Troubleshooting as well as improvement in efficiency and performance is typically achieved by trial and error based on past experience. Failure of chemical process equipment can result in undesirable downtime and loss of revenue. Hence, more adequate techniques of troubleshooting are required so that downtime can be minimized. Computational fluid dynamics has been identified as a viable solution method for analyzing complex flows in complex systems.
Multiphase Flows:
Multiphase flow refers to a situation where more than one fluid is present and the fluids are immiscible. The term 'phase' is used in a much wider sense and does not necessarily refer to thermodynamic phases, viz. solid, liquid, gas but refers to multiple fluids where the fluids are mixed at a macroscopic level, the mixing scale is larger than the molecular scale. For ease of discussion only two-phase flow systems will be discussed but the concepts and conclusions apply to systems having three or more phases as well. Multiphase flows can be broadly classified into continuous-dispersed flows and continuous-continuous flows. Continuous-dispersed flows are those where the primary phase is continuous, the secondary phase is discontinuous and dispersed within the
primary phase. The dispersed phase occupies disconnected regions of space and is present in the form of drops, bubbles or particles. Flow of slurries, bubbles and particulate flows are some examples of continuous-dispersed flows. Continuouscontinuous flows are those where all fluids are continuous. Flows involving a free surface between fluids is an example of such a situation.
A multiphase flow system consists of multiple phases occupying the same region of space. Complex interactions arise due to the proximity of multiple phases. The fluids compete for the same volume in space. The difference in fluid properties between the phases results in mass, momentum and energy exchange between the phases. Models that describe these interactions are complex and sophisticated.
CFD Models for Multiphase Flows:
CFD methods are based on first principles of mass, momentum and energy conservation as described by the Navier-Stokes equations. These methods involve the solution of conservation equations of mass, momentum, energy and species at thousands of locations within the flow domain. The computed solution provides flow variables such as velocity, pressure, temperature, density, concentration etc. at thousands of locations within the domain. CFD models for multiphase flows can be broadly divided into the following categories: Algebraic slip model, Drift flux model, Eulerian-Lagrangian models and EulerianEulerian models. In each of the above methods the conservation equations of mass, momentum and energy are solved. The presence of each phase is quantified by volume fraction; which represents the fraction of volume occupied by that particular phase. Volume fraction is obtained by solving individual continuity equations for each phase. Algebraic Slip Model: This is the simplest multiphase flow model and is essentially a single-phase model. This model is suitable for continuous-dispersed systems. It is based on the assumption of interpenetrating fluids, where there is no interface between the fluids and the two phases can move at different velocities. The phases are modeled by solving one set of continuity and momentum equations using average or mixture properties for density and viscosity. The relative velocity between the phases, also known as slip velocity is defined using an algebraic relationship. Local momentum equilibrium between the phases is assumed to prescribe the slip velocity between the phases. The distribution of the dispersed phase is described by its volume fraction. This is computed by solving a continuity equation for the dispersed phase. This model is suitable for those situations where a large number of dispersed phases are present and a full multiphase solution is not possible. This model is valid only for those situations where the sum total of volume fractions of all dispersed phases is very small.
Drift Flux Model: This model can be referred to as a one-and-half phase model. This model is applied for continuous-dispersed systems and is based on the assumption of interpenetrating fluids. The phases are modeled by solving one set of continuity and momentum equations using average or mixture properties for density and viscosity. The relative velocity between the phases is computed using an algebraic relationship and is based on the assumption of local momentum equilibrium. This occurs when the relative velocity between phases, also known as drift, is small and the inertia associated with drift can be neglected. The distribution of the dispersed phase is described by its volume fraction and is computed by solving a continuity equation for the dispersed phase. This model accounts for the volume displaced by the dispersed phase and is thus less restrictive than the algebraic slip model.
Eulerian-Lagrangian Model: This model is applicable to continuous-dispersed systems and is very often referred to as a discrete particle model or particle transport model. The primary phase is continuous, which may be a gas or a liquid. The secondary phase is discrete and may be composed of particles, drops or bubbles. The continuous phase flow field is computed by solving the Navier-Stokes equations. Flow trajectories, heat and mass transfer from and to the discrete phase are computed by solving discrete equations for the dispersed phase. The dispersed phase is represented by tracking a small number of representative particle streams. For each particle stream ordinary differential equations representing mass, momentum and energy transfer are solved to compute its state and location. The two phases are coupled by including appropriate interaction terms in the continuous phase equations. The volume displaced by the dispersed phase is not taken into account. As a result, this model is applicable for low volume fractions of the dispersed phase, typically less than 10%. This model is applicable for those situations where the discrete phase is injected as a continuous stream into the continuous phase. Equations for the dispersed phase: A force balance equation based on Newton's second law of motion is solved to compute the trajectory of the discrete phase.
du p dt
where m is the particle mass, u p is the particle velocity and F is the force acting on the particle and t is time. The total force acting on the particle is composed of various forces such as drag, gravity, buoyancy, pressure gradient, virtual mass force, lift, thermophoretic force; any other significant force may also be included. Drag, gravity and buoyancy are typically the most dominant forces on a particle. Drag force for spherical particles can be computed through well-known correlations. Correlations for spherical particles are applied to estimate the drag force. If the particle is non-spherical, corrections to the drag force computed using correlations for spherical particles are applied. If the continuous
phase flow field is turbulent then turbulent interactions between the particles and the turbulent eddies in the continuous phase can be modeled using a stochastic model. Heat transfer to the particle is modeled by solving a lump capacity energy balance equation.
mC p
dT = Q c + Q r + Qm dt
Where C p is the particle specific heat, T is particle temperature and Qc is heat transfer due to convection, Qr is heat transfer due to radiation and Qm is heat transfer due to mass transfer.
Qc = hA(T f − T )
Where h is heat transfer coefficient and is computed using correlations for spherical particles. A is area of particle. T f is local temperature of the continuous phase.
Qr = σA(αT∞ − εT 4 )
Where σ is boltzman constant, α is absorption coefficient, ε is emissivity and T∞ is the surrounding medium temperature.
Qm = dm L dt dm is rate of mass transfer and L is latent heat of vaporization. dt
Mass transfer between the particle and continuous phase is modeled using the following equation
dm = K m (C f − C ) dt
Where K m is mass transfer coefficient, C is concentration of evaporating specie component in particle and C f is concentration of evaporating specie component in fluid. If the volatile components of the particle are boiling a more sophisticated relationship for mass transfer is applied. The Eulerian-Lagrangian model is applied to simulate flows in unit operations where the volume fraction of the dispersed phase is small, such as in cyclones, precipitators and spray dryers. This model provides complete information on the behavior and residence
time of individual particles. Interaction of individual particle streams with turbulent eddies and solid surfaces such as walls can be modeled.
Eulerian-Eulerian Model: This is the most general model for multiphase flows. It is based on the principal of inter-penetrating continua. Each phase is governed by the same set of governing equations, viz. the Navier-Stokes equations. The phases share the same volume, penetrate each other in space and exchange mass, momentum and energy with each other. Each phase is described by its distinctive physical properties and has its own velocity, pressure, concentration and temperature field. For ease of discussion, mathematical formulation for two-phase systems is presented below. Concepts and conclusions apply for multiple phases as well. A general transport equation for EulerianEulerian model is as follows.
d ( ρ1r1φ1 ) + ∇.( ρ1r1U 1φ1 ) = ∇.( r1Γ1∇φ1 ) + Sp + IP12 dt
Where subscript 1 refers to phase 1, ρ is density of phase, r is volume fraction, U is velocity, φ is any conserved scalar. If φ is one then the above equation represents volume fraction equation i.e. mass conservation for that phase. If φ is the velocity vector and Sp is pressure gradient then the equation represents momentum transfer. The first term on the left-hand-side of equation (A.7) represents temporal change of scalar φ at a fixed point in space, the second term represents change in φ due to convection, the first term on right-hand-side represents diffusion, the second term on the right-hand-side represents source terms i.e. generation or destruction of φ due to reactions or any other mechanism. The last term IP12 represents interaction between the phases and is normally referred to as the interphase transfer term and is represented as follows.
IP12 = k12 (φ 2 − φ1 ) + m12φ 2 − m21φ1
The first term in equation (A.8) represents interphase transfer due to difference in φ between the phases. If φ is velocity, then this term represents momentum transfer due to difference in velocity and, if φ is temperature, then it represents heat transfer due to difference in temperature. The second and third terms represent interphase transfer due to mass transfer. The interphase transfer coefficient k12 is computed using empirical correlations. The Eulerian-Eulerian model is applicable for continuous-dispersed as well as continuous-continuous systems. For continuous-dispersed systems the velocity of each phase is computed using the Navier-Stokes equations. The dispersed phase may be in the form of particles, drops or bubbles. The forces acting on the dispersed phase are modeled using empirical correlations and included as part of the interphase transfer terms. Drag, lift, gravity, buoyancy, virtual mass effects are some of the forces that may be acting on the dispersed phase. These forces are computed for an individual particle and then scaled
by the local volume fraction to account for multiple particles. If the dispersed phase is in the form of bubbles, then appropriate correlations for bubble distortion effects are also required. Correlations based on a single particle are not appropriate when the local volume fraction of the dispersed phase is high. Multi-particle effects and corrections based on the presence of multiple particles in the vicinity of a single particle are applied. Simulation of gas-solid flows requires additional models. Gas-solid flows can be classified into three regimes: • Elastic regime: in this regime the solid phase supports large loads and is normally at its maximum packing condition. • Plastic regime: in this regime the solid phase flows as a plastic material. Flow of solids is not continuous but in the form of bands or layers. • Viscous regime: this regime is characterized by free flowing solids as found in risers and fluidized beds. Current CFD methods are applicable for viscous regime flows. General models for multiphase flows are not suitable for gas-solid flows as these models do not include effects that are dominant in gas-solid flows but are not important in liquid-liquid, gasliquid, solid-liquid systems. In gas-solid flows, particle-particle interaction plays an important role and results in additional forces in the solid phase. These forces are modeled either using empirical solids pressure type of models or using a more sophisticated approach based on kinetic theory. Continuous-continuous systems are modeled using a special version of the EulerianEulerian model known as the homogenous flow model or the volume of fluid model. This model is appropriate if the interphase drag is large and the phases attain equilibrium over small length scales. In this model velocity field for both phases is assumed to be the same and a single set of momentum equations with average fluid properties is solved. Individual volume fraction equations are solved to track the phases. This model is typically applied to simulate free surface flows, filling of containers, formation of bubbles, drops and breakup of jets. Surface tension effects are typically included as part of this model.
Multiphase Flow Applications:
The CFD models described above are applied to simulate multiphase flows in a wide variety of process units. CFD solutions are used to take an 'inside look' into the operation of these devices. This results in a detailed understanding of the flow behavior, providing guidance for process improvement and increased efficiency. In many cases CFD solutions are obtained to plan design changes and verify design change concepts. This results in minimization of down-time and increased productivity.
CFD technology has made numerous advances over the past few years. It can now be applied to study complex flow fields such as multiphase flows in chemical process units. Successful simulation of complex multiphase phenomena requires full understanding of the underlying models. Limitations and assumptions associated with these models play a critical role in judicious choice of models. Applicability of CFD techniques for design, analysis, optimization and process improvement of various unit operations has been discussed. The applications discussed in the above sections show only a portion of the wide range of applications for multiphase CFD in the chemical process industries. The full potential of CFD for multiphase flow applications is yet to be fully realized.