Starting Fluent/Gambit from UNIX Logon using your userID and password Toggle K+ / non-KDE Apps / X Terminal to get a x term window Or toggle on the low bar the display icon to get a x term window Write: >module add fluent gambit This will start Gambit Write: >module add fluent fluent This will start Fluent Your work will be saved in your directory so it’s possible to reach the files also from PC. Starting Fluent/Gambit from PC Logon using your userID and password Toggle start and All programs Choose Fluent Inc. products/ Fluent 6.1/ Fluent 6.1 Toggle start and run Write gambit PS for the moment it’s NOT possible to run gambit on PC, workstations are needed.
1.2 Program Structure
Example 2 seconds6 seconds 15 seconds 27 seconds
50 seconds 200 seconds 100 seconds
1.3 Program Capabilities The FLUENT solver has the following modeling capabilities: flows in 2D or 3D geometries using unstructured solution-adaptive triangular/tetrahedral, quadrilateral/hexahedral, or mixed (hybrid) grids that include prisms (wedges) or pyramids. (Both conformal and hanging-node meshes are acceptable.) incompressible or compressible flows steady-state or transient analysis inviscid, laminar, and turbulent flows convective heat transfer, including natural or forced convection coupled conduction/convective heat transfer radiation heat transfer chemical species mixing and reaction, including combustion Lagrangian trajectory calculations for a dispersed phase of particles/droplets/bubbles, including coupling with the continuous phase phase-change models flow through porous media multiphase flows, including cavitation These capabilities allow FLUENT to be used for a wide variety of applications, including the following: Process and process equipment applications Power generation and oil/gas and environmental applications Aerospace and turbomachinery applications Automobile applications Heat exchanger applications Electronics/HVAC/appliances Materials processing applications Architectural design and fire research
1.4.1 Planning Your CFD Analysis When you are planning to solve a problem using FLUENT, you should first give consideration to the following issues: Definition of the Modeling Goals: What specific results are required from the CFD model and how will they be used? What degree of accuracy is required from the model? Choice of the Computational Model: How will you isolate a piece of the complete physical system to be modeled? Where will the computational domain begin and end? What boundary conditions will be used at the boundaries of the model? Can the problem be modeled in two dimensions or is a three- dimensional model required? What type of grid topology is best suited for this problem? Choice of Physical Models: Is the flow inviscid, laminar, or turbulent? Is the flow unsteady or steady? Is heat transfer important? Will you treat the fluid as incompressible or compressible? Are there other physical models that should be applied? Determination of the Solution Procedure: Can the problem be solved simply, using the default solver formulation and solution parameters? Can convergence be accelerated with a more judicious solution procedure? Will the problem fit within the memory constraints of your computer, including the use of multigrid? How long will the problem take to converge on your computer? Careful consideration of these issues before beginning your CFD analysis will contribute significantly to the success of your modeling effort.
1.4.2 Problem Solving Steps Once you have determined the important features of the problem you want to solve, you will follow the basic procedural steps shown below. 1. Create the model geometry and grid. 2. Start the appropriate solver for 2D or 3D modeling. 3. Import the grid. 4. Check the grid. 5. Select the solver formulation. 6. Choose the basic equations to be solved: laminar or turbulent (or inviscid), chemical species or reaction, heat transfer models, etc. Identify additional models needed: fans, heat exchangers, porous media, etc. 7. Specify material properties. 8. Specify the boundary conditions. 9. Adjust the solution control parameters. 10. Initialize the flow field. 11. Calculate a solution. 12. Examine the results. 13. Save the results. 14. If necessary, refine the grid or consider revisions to the numerical or physical model. Step 1 of the solution process requires a geometry modeler and grid generator. We will use GAMBIT for geometry modeling and grid generation Single-Precision and Double-Precision Solvers Both single-precision and double-precision versions of FLUENT are available on all computer platforms. For most cases, the single-precision solver will be sufficiently accurate, but certain types of problems may benefit from the use of a double-precision version.
Control volume Mesh/grid created in GAMBIT Using the conservation laws for mass, momentum and energy for each CV (stationary conditions)
Integration of these equations on the individual control volumes to construct algebraic equations for the discrete dependent variables (``unknowns'') such as velocities, pressure, temperature and so on. Linearization of the discretized equations and solution of the resultant linear equation system to yield updated values of the dependent variables. FLUENT provides three different solver formulations: segregated coupled implicit coupled explicit The segregated and coupled approaches differ in the way that the continuity, momentum, and (where appropriate) energy and species equations are solved: the segregated solver solves these equations sequentially (i.e., segregated from one another), while the coupled solver solves them simultaneously (i.e., coupled together). Both formulations solve the equations for additional scalars (e.g., turbulence or radiation quantities) sequentially. The implicit and explicit coupled solvers differ in the way that they linearize the coupled equations.
Segregated Solution Method Using this approach, the governing equations are solved sequentially (i.e., segregated from one another). Because the governing equations are non-linear (and coupled), several iterations of the solution loop must be performed before a converged solution is obtained. Each iteration consists of the steps outlined below: 1. Fluid properties are updated, based on the current solution. (If the calculation has just begun, the fluid properties will be updated based on the initialized solution.) 2. The u, v, and w momentum equations are each solved in turn using current values for pressure and face mass fluxes, in order to update the velocity field. 3. Since the velocities obtained in Step 2 may not satisfy the continuity equation locally, a ``Poisson-type'' equation for the pressure correction is derived from the continuity equation and the linearized momentum equations. This pressure correction equation is then solved to obtain the necessary corrections to the pressure and velocity fields and the face mass fluxes such that continuity is satisfied. 4. Where appropriate, equations for scalars such as turbulence, energy, species, and radiation are solved using the previously updated values of the other variables. 5. When interphase coupling is to be included, the source terms in the appropriate continuous phase equations may be updated with a discrete phase trajectory calculation. 6. A check for convergence of the equation set is made. These steps are continued until the convergence criteria are met. U-velocity is calculated in all CV, then v-velocity is calculated in all CV …..
Coupled Solution Method The coupled solver solves the governing equations of continuity, momentum, and (where appropriate) energy and species transport simultaneously (i.e., coupled together). Governing equations for additional scalars will be solved sequentially (i.e., segregated from one another and from the coupled set. 1. Fluid properties are updated, based on the current solution. 2. The continuity, momentum, and (where appropriate) energy and species equations are solved simultaneously. 3. Where appropriate, equations for scalars such as turbulence and radiation are solved using the previously updated values of the other variables. 4. When interphase coupling is to be included, the source terms in the appropriate continuous phase equations may be updated with a discrete phase trajectory calculation. 5. A check for convergence of the equation set is made. These steps are continued until the convergence criteria are met.
SUMMARY The segregated approach solves for a single variable field ( p) by considering all cells at the same time. It then solves for the next variable field by again considering all cells at the same time, and so on. The coupled implicit approach solves for all variables ( p, u, v, w, T) in all cells at the same time. The coupled explicit approach solves for all variables ( p, u, v, w, T) one cell at a time
FLUENT stores discrete values of the variables at the cell centers ( c0 and c1 in Figure). However, face values are required for the convection terms and must be interpolated from the cell center values. This is accomplished using an upwind scheme. Upwinding means that the face value is derived from quantities in the cell upstream, or ``upwind,'' relative to the direction of the normal velocity. FLUENT allows you to choose from several upwind schemes: first-order upwind, second-order upwind, power law, and QUICK First-Order Upwind Scheme When first-order accuracy is desired, quantities at cell faces are determined by assuming that the cell-center values of any field variable represent a cell-average value and hold throughout the entire cell; the face quantities are identical to the cell quantities. Thus when first-order upwinding is selected, the face value is set equal to the cell-center value of in the upstream cell Second-Order Upwind Scheme When second-order accuracy is desired, higher-order accuracy is achieved at cell faces through a Taylor series expansion of the cell-centered solution about the cell centroid Under-Relaxation Because of the nonlinearity of the equation set being solved by FLUENT, it is necessary to control the change of . This is typically achieved by under-relaxation, which reduces the change of produced during each iteration. In a simple form, the new value of the variable within a cell depends upon the old value,, the computed change in, , and the under- relaxation factor, , as follows:
Judging Convergence There are no universal metrics for judging convergence. Residual definitions that are useful for one class of problem are sometimes misleading for other classes of problems. Therefore it is a good idea to judge convergence not only by examining residual levels, but also by monitoring relevant integrated quantities such as drag or heat transfer coefficient. For most problems, the default convergence criterion in FLUENT is sufficient. This criterion requires that the scaled residuals decrease to for all equations except the energy and P-1 equations, for which the criterion is At the end of each solver iteration, the residual sum for each of the conserved variables is computed and stored, thus recording the convergence history. This history is also saved in the data file. The residual Rf computed by FLUENT's segregated solver is the imbalance summed over all the computational cells P. This is referred to as the ``unscaled'' residual In general, it is difficult to judge convergence by examining the residuals. FLUENT scales the residual using a scaling factor representative of the flow rate of f through the domain. For the continuity equation, the unscaled residual for the segregated solver is defined as The segregated solver's scaled residual for the continuity equation is defined as The denominator is the largest absolute value of the continuity residual in the first five iterations.
Step-by-Step Solution Processes One important technique for speeding convergence for complex problems is to tackle the problem one step at a time. When modeling a problem with heat transfer, you can begin with the calculation of the isothermal flow. To solve turbulent flow, you might start with the calculation of laminar flow. When modeling a reacting flow, you can begin by computing a partially converged solution to the non-reacting flow, possibly including the species mixing. When modeling a discrete phase, such as fuel evaporating from droplets, it is a good idea to solve the gas-phase flow field first. Such solutions generally serve as a good starting point for the calculation of the more complex problems. These step-by-step techniques involve using the Solution Controls panel to turn equations on and off.