Using the Segregated and Coupled Solvers

Outline Introduction Solution procedure Terminology Convergence What is convergence? Judging and monitoring convergence Accelerating convergence Stability Accuracy Discretization schemes Grid adaption Grid independence

Introduction FLUENT 5 provides two classes of numerical methods Segregated solver (FLUENT/UNS, FLUENT 4.5) Coupled solver Explicit (RAMPANT) Implicit Can switch “on-the-fly” between these methods Solution procedure that you follow is basically the same for all solvers. Both classes of methods employ similar discretization schemes (finite-volume) but different linearization and solution methods

Linearization: Implicit vs. Explicit Discrete nonlinear governing equations need to be linearized so that system of equations can be solved for dependent variables in the cells Implicit linearization - unknown value in each cell uses existing and unknown values from neighboring cells System of equations obtained which must be solved simultaneously In segregated approach, each variable equation linearized implicitly with respect to itself; variable field solved over all cells In coupled approach, each equation in coupled set linearized implicitly with respect to all dependent variables; block coupled equations solved Explicit linearization - unknown value in each cell computed from relations that include only existing values Each equation in coupled set linearized explicitly Multi-stage (Runge-Kutta) solver can be used

Solution Procedure: What You Do Set the solution parameters Initialize the solution Enable the solution monitors of interest Calculate a solution Modify solution parameters or grid Check for convergence No Yes Check for accuracy No Yes Stop

Segregated Solution Procedure: What the Solver Does Update properties. Solve momentum equations (u, v, w velocity). Solve pressure-correction (continuity) equation. Update pressure, face mass flow rate. Solve energy, species, turbulence, and other scalar equations. Converged? No Yes Stop

Coupled Solution Procedure: What the Solver Does Update properties. Solve continuity, momentum, energy, and species equations simultaneously. Solve turbulence and other scalar equations. Converged? No Yes Stop

Unsteady Solution Procedure Same procedure for segregated and time-implicit coupled solvers: Execute segregated or coupled procedure, iterating to convergence Take a time step Requested time steps completed? No Yes Stop Update solution values with converged values at current time Time-explicit coupled solver explicitly solves for all variables one cell at a time at each time step (Runge-Kutta).

What is Convergence? At convergence: All discrete conservation equations (momentum, energy, etc.) are obeyed in all cells to a specified tolerance. Solution no longer changes with more iterations. Overall mass, momentum, energy, and scalar balances are obtained. “Residuals” measure imbalance (or error) in conservation equations. The governing transport equations are solved iteratively. Final solution (ideal): Iteration i: Opposite of convergence is divergence. Imbalance grows larger with more iterations. Note: Convergence is not the same as accuracy!

Judging Qualitative Convergence Generally, a decrease in residuals by 3 orders of magnitude (tolerance=110-3 ) indicates at least qualitative convergence. Major flow features established Exceptions: In segregated solver scaled energy residual must decrease to 110-6. Scaled species residual may need to decrease to 110-5 to achieve species balance. Monitor other variables and balances to ensure quantitative convergence. Beware: Unconverged results can be misleading!

Residual Plots Residual plots show: When the residual values have reached the specified tolerance Which equations are having convergence trouble continuity equation convergence trouble affects convergence of all equations all equations converged

Monitoring Quantitative Convergence In addition to residuals, you can also monitor: Lift, drag, or moment Solve  Monitors  Force... Value of a variable or function: At a boundary On a defined surface At a point Solve  Monitors  Surface... When the monitored value stops changing, the solution is converged. Monitoring average static temperature over a surface

Convergence Monitor Plots When lift value levels off, solution is converged.

Checking Balances In addition to monitoring residual and variable histories, you should also check for overall heat and mass balances. Net imbalance should be less than 0.1% of net flux through domain. Report  Fluxes...

Decreasing the Convergence Tolerance Recall: at convergence, all discrete conservation equations are obeyed in all cells to a specified tolerance. If your residuals indicate that the solution is converged, but the solution is still changing or has a large mass/heat imbalance: Try reducing the convergence tolerance. Solve  Monitors Residual... Then calculate until solution converges to the new tolerance.

Accelerating Convergence Convergence can be accelerated by: Supplying good initial conditions Modifying under-relaxation parameters or changing the Courant number (coupled solver) Controlling multigrid solver settings

Supplying Initial Conditions Initialize all solution variables before calculating a solution. Solve  Initialize  Initialize... Also improves solution stability In some cases, correct initial guess is required: Example: nozzle will not attain supersonic flow unless initial flow condition is supersonic. “Patch” values for individual variables in certain regions. Solve  Initialize  Patch... Free jet flows (patch high velocity for jet) Combustion problems (patch high temperature for ignition) Start from a previous solution. Often used in conjunction with patching.

Starting from a Previous Solution Previous solution can be used as an initial condition when changes are made to problem definition.

What is Under-relaxation? Equation set being solved is non-linear. Equation for one variable may depend on other variables, e.g., Temperature Mass fraction For solver stability, the change in a variable’s value between iterations is reduced by an “under-relaxation” factor, : e.g., under-relaxation of 0.2 limits the change in P to 20% of the computed change of  for one iteration. Under-relaxation factors for equations outside coupled set (for coupled solver) are set just as in segregated solver

Modifying Under-relaxation Factors Use default under-relaxation parameters to start a calculation. To accelerate convergence, increase under-relaxation factor for an equation if its residual is either: Monotonically decreasing Oscillating very slightly, but decreasing Solve  Controls  Solution... Increasing under-relaxation factors can also create instability! Leads to divergence! Good idea to save intermediate data before increasing under-relaxation.

Example: Accelerating Convergence Residual plot showing good convergence behavior accelerated by an increase in under-relaxation: Under-relaxation increased here

The Multigrid Solver “Multigrid” solver accelerates convergence for: Large number of cells Large cell aspect ratios x/y > 20 or so, for example Large differences in thermal conductivity Such as in conjugate heat transfer General concept of multigrid is the same for structured and unstructured grids, although the implementation is different.

The Multigrid Concept (1) Multigrid solver uses sequence of grids going from fine to coarse. You choose the number of coarse grid levels. Solver creates them automatically. Influence of boundaries and far-away points more easily transmitted to interior on coarse meshes than on fine meshes. In coarse meshes, grid points closer together in computational space. Fewer computational cells between any two spatial locations. However, fine meshes give more accurate solutions. original grid coarse grid level 1 coarse grid level 2

The Multigrid Concept (2) Use solution on coarse meshes as starting point for solution on finer meshes. Coarse-mesh solution contains influence of boundaries and far neighbors. These effects felt more easily on coarse mesh. Accelerates convergence on fine mesh Final solution obtained for mesh you created. Coarse mesh calculations: Only speed up convergence Do not change final answer fine mesh corrections summed equations (or volume-averaged solution) coarse mesh

Courant Number for Coupled Solver Time step t computed from CFL (Courant-Friedrichs-Lewy) condition: In general, for coupled/explicit solver: Courant number cannot be > 2.0 from stability constraints; default = 1.0. May have to be set lower for problems with complex physics (e.g., high Mach number). Defines time step t for time-explicit unsteady solver. For coupled/implicit solver: Courant number can be set to 10, 100, or even higher Multigrid solver can reduce CFL if divergence is detected CFL = Courant number where u = appropriate velocity scale x = grid spacing

Increasing the Courant Number To accelerate convergence, increase the Courant number if all residuals are either: Monotonically decreasing Oscillating very slightly, but decreasing Solve  Controls  Solution...

Stability If residuals are increasing or “stuck,” less aggressive solver settings are needed. Try one or more of these changes: Decrease under-relaxation for equation(s) having convergence trouble. (segregated solvers) Reduce Courant number (coupled solver). Adjust multigrid parameters. Try to compute an initial solution with a first-order discretization scheme.

Example: Improving Stability Residual plot showing poor convergence behavior improved by a decrease in under-relaxation: Under-relaxation decreased here

Accuracy Once you have a converged solution, need to be sure it is accurate. Compute converged solution. Increase to second-order discretization scheme (if not already), and recalculate a converged solution. Examine results for significant flow features or variables. Refine grid and recalculate a converged solution. Compare results w/results for last grid. Solution is grid-independent! Solution different? Yes No

Choosing the Discretization Scheme First-order: computes values at faces using values at adjacent cells. Faster convergence; less accurate Second-order: computes face values using values at adjacent cells and their neighbors. Slower convergence; more accurate Provides more accurate results, especially for tri/tet meshes. When flow is not aligned with the grid, first-order scheme increases discretization error. In general, you should try to obtain a second-order solution. face adjacent cells

Grid Adaption In general, finer grid = more accurate solution. Grid adaption allows you to add more cells where they are needed to resolve the flow field. Example: regions of rapidly-changing velocity or pressure If converged solution is not accurate enough: Adapt grid in appropriate region(s). Then continue calculation to convergence. Use solution on original grid as initial solution. Data from original grid is automatically interpolated to finer grid. Repeat adaption/calculation procedure if necessary. When solution no longer changes with further grid adaption, you have a “grid-independent” solution.

Example: Supersonic Flow Over a Cylinder Adapt grid in regions of high pressure gradient because there is a jump in pressure across the shock. Adapt  Gradient... Original mesh Mesh after pressure gradient adaption

Example: Impinging Jet Adapt grid in regions of high x velocity. Adapt  Iso-Value... Original mesh shown with contours of x velocity Mesh after x-velocity isovalue adaption

Adaption Guidelines In general, avoid large volume variations in regions with large gradients. If you know where gradients are expected (e.g., shock, boundary layer), concentrate the original grid in that region. If you need to adapt in a region with a large gradient, try to adapt uniformly.

Determining Grid Independence Compare results obtained w/different grids to determine grid independence: Overall pressure drop (Report  Surface Integrals...) Overall heat transfer coefficient (Report  Surface Integrals...) Lift, drag, and moment coefficients (Report  Forces...) Average value of a variable at a point or on a surface (Report  Surface Integrals...) Average exit pressure, temperature at a significant location, etc. Variation of a variable value along a line (Plot  XY Plot...) Flow behaving “as expected” (use numerical and graphical reports)

Summary Solution procedure for the segregated and coupled solvers is the same: Calculate until you get a converged solution. Obtain second-order solution (recommended). Refine grid and recalculate until grid-independent solution is obtained. All solvers provide tools for judging and improving convergence and ensuring stability. All solvers provide tools for checking and improving accuracy. Solution accuracy will depend on the appropriateness of the physical models that you choose and the boundary conditions that you specify.