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 many problems, the default convergence criterion in Ansys Fluent is sufficient. This criterion requires that the globally scaled residuals, defined by Equation 36–28, Equation 36–32, or Equation 36–35 decrease to for all equations except the energy and P-1 equations, for which the criterion is .

Sometimes, however, this criterion may not be appropriate. For example:

When issues like the above arise, you should consider using locally scaled residuals defined by Equation 36–29, Equation 36–31, or Equation 36–36, which have a default convergence criterion for all equations of 10^-5 and 10^-4 for steady-state flows and transient flows, respectively. Experience suggests that locally scaled residuals may be more universal for the purposes of judging convergence than globally scaled residuals. Note that you may want to adjust the convergence criterion from the default value for the locally scaled continuity residual based on your specific application.

Another popular approach to judging convergence is to require that the unscaled residuals drop by three orders of magnitude. Ansys Fluent provides residual normalization for this purpose, as discussed in Definition of Residuals for the Pressure-Based Solver, where residuals are defined for both the pressure-based solver and the density-based solver. In this approach the convergence criterion is that the normalized unscaled residuals should drop to . However, this requirement may not be appropriate in many cases:

Regardless of the residual scaling method, it is wise to monitor important solution quantities, such as drag or overall heat transfer coefficient, before concluding that the solution has converged.

Conversely, it is possible that if the initial guess is very bad, the initial residuals are so large that a three-order drop in residual does not guarantee convergence. This is specially true for and equations where good initial guesses are difficult. Here again it is useful to examine overall integrated quantities that you are particularly interested in. If the solution is unconverged, you may drop the convergence tolerance, as described in Modifying Convergence Criteria.

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 Task Page to turn equations on and off in the Equations dialog box.

The default algebraic multigrid settings are appropriate for nearly all problems, but in rare cases you may need to make minor adjustments. Setting Algebraic Multigrid Parameters describes how to analyze the multigrid solver’s performance to determine which parameters.

It is possible to make several changes to the multi-stage time-stepping scheme itself. See Changing the Multi-Stage Scheme for detailed information.

Poor quality meshes are meshes containing highly skewed cells, highly non-orthogonal cells, non-convex cells, or cells with left-handed faces. Such mesh elements tend to decrease the numerical stability of traditional CFD discretization algorithms. These mesh elements require special treatment, namely, a numerical correction of the transport equation discretization, which is intended to improve the numerical properties of the solution algorithms at mesh cells of poor quality. This correction is referred to as "poor mesh numerics", and it is enabled by default so that it is applied to cells with an orthogonal quality of 0.

If you read in a poor quality mesh containing cells and faces with corrupt metrics, you will see a warning in the console of the following form:

Info: The mesh contains elements that are invalid or of poor quality.
      A different numerical scheme will be applied to these elements,
      which may affect the quality of the solution. It is recommended
      that you consider removing the invalid and poor quality elements
      in the mesh.
      For more information on the invalid and poor quality elements,
      please use the following TUI commands:
      /mesh/check
      /mesh/repair-improve/report-poor-elements.

For details on the tools available for investigating corrupt cells and faces and repairing them, see Repairing Meshes. For the poor quality cells that cannot be repaired, you can rely on the application of poor mesh numerics to allow you to proceed.

The local solution correction applied by poor mesh numerics can be of 0th, 1st, or 2nd order:

In other words, the discretization error will be independent of the mesh size in this region if 0th order is used. It will decrease linearly with subsequent grid refinement when 1st order is used, and quadratically when the 2nd order option is selected.

It is strongly recommended that you use the default 1st order solution correction, which provides a reasonable compromise between accuracy and stability gain. When only a few cells are invalid, you can attempt to use the other schemes: for meshes of better (and yet still low) quality, you can try the 2nd order option, which will preserve the mesh convergence behavior provided by the convection term discretization schemes; if no convergence is obtained with any of the aforementioned schemes, you can try the 0th order option, which will provide the highest stability and at the same time the lowest accuracy. Note that in regions with highly nonlinear flow physics, the 0th order scheme can yield highly nonphysical results. To change the order scheme, use the prompt in the following text command: solve/set/poor-mesh-numerics/enable?.

The three solution correction schemes should be applied to only a small percentage of the mesh cells, in order to strike a balance between the robustness of the solution and solution efficiency. The computational time (or cost or run time requirements) for all three order schemes will increase linearly as the number of cells identified as poor quality cells increases. Provided that there is reasonable convergence behavior with all three schemes, the 1st order option will be the fastest; 0th and 2nd order schemes will have similar run times to each other. If a large percentage of the cells are marked for correction due to poor quality metrics, then it is highly recommended that you abandon the mesh for one with better quality metrics.

If the default poor mesh numerics settings are not sufficient to provide stability for your mesh, you can enable the following text command so that the cell centroids of poor cells are relocated with the goal of enhancing the orthogonality metrics: solve/set/poor-mesh-numerics/orthogonality-enhancing-cell-centroids?. This can be used with all mesh types, and is applied to cells when the criterion value is equal to or less than a threshold value defined as part of the text command. Increasing the threshold for the orthogonal quality can increase solver robustness, but at the cost of reduced solution accuracy. Note that the enhanced metrics are only apparent when reporting the quality in the solution mode of Fluent, and not in the meshing mode.

If you continue to have stability problems, you can increase the range of cells to which the poor mesh numerics correction is applied. As stated previously, when the solve/set/poor-mesh-numerics/enable? text command is enabled, only cells with an orthogonal quality of 0 are corrected by default; this is a conservative setting, and can be changed by enabling the following text commands:

When you initialize or read data for a case with non-premixed or partially premixed combustion, a register-based definition for poor mesh numerics named pmn_pdf_stability_marker is automatically created. This definition is deactivated by default; if activated, it may increase the robustness of combustion simulations that use a PDF table. For further details, see Enabling Robust Numerics for Combustion with a PDF Table.

Note that when using register-based definitions for poor mesh numerics, the reporting of poor mesh element statistics (using the mesh/repair-improve/report-poor-elements text command) will also include the cells added from the registers, as well as their neighboring cells, resulting in an overall larger number of cells being identified. For example:

Poor Mesh Element Statistics:
Identified    0 faces with too small area.
Identified    0 faces adjacent to negative volume cells.
Identified    0 faces adjacent to bad quality cells.
Identified   43 cells from register-based poor mesh numerics and neighbors.

There are additional text commands that can be useful when applying poor mesh numerics, which are defined as follows:

The warped-face gradient correction (WFGC) is designed to improve gradient accuracy for all gradient methods—cell based, node based and least squares based gradients. WFGC is recommended for 3D simulations on polyhedral, hexahedral, and hybrid meshes (meshes containing a mix of hexahedral and polyhedral cells), and it is enabled by default when you read a mesh that contains polyhedra (note that if you append a mesh that contains polyhedra to a mesh that doesn't, you would have to enable WFGC manually in the Solution Methods task page if you want to use it). Note that these types of mesh cells may not have perfectly planar faces, which can affect the overall accuracy of the Green Gauss surface integral. WFGC is also recommended when you encounter numerical difficulties in simulations that involve a mesh that has large differences in the volumes of neighboring cells, such as hex cells with hanging node interfaces.

WFGC computations aim to resolve gradient accuracy degradation due to very high aspect ratio, cells with non-flat faces in the boundary layer, and highly deformed cells where the formal cell centroid lies outside of the control volume.

WFGC has two modes, fast mode and memory saving mode. Fast mode does not increase gradient computation time for static meshes (except for cases that use the Green-Gauss Node Based gradient method with a turbulence model), but it does require additional memory. There is roughly a 22% increase in memory for a basic flow solution, but this additional overhead does not change as more models (turbulence, species transport, radiation, and so on) are enabled. Memory saving mode does not increase memory consumption, but it slows down iteration execution time for static and dynamic meshes.

Numerical noise can arise in the energy solution field when there are large variations in properties at certain locations, such as the heat capacity at coupled walls or the combustion variables in cases with phase change. With the use of high-order discretization, the numerical noise remains in the solution fields, which contaminates the solution and may lead to divergence. An energy equation numerical noise filter is available for the pressure-based solver, which aims to remove the numerical noise from the domain by applying a mathematical extrema condition in the numerical noise region. This process slightly reduces accuracy in those regions, but increases the robustness of the calculation. The numerical noise filter is not applied after the numerical noise is removed from the region, in order to regain high-order accuracy. To enable / disable the energy equation numerical noise filter, use the following text command:

solve → set → advanced → energy-numerical-noise-filter

Note that the energy equation numerical noise filter is not enabled by default. For problematic cases where the energy equation diverges or generates non-physical results, it is recommended that you use this filter from the start of the simulation, rather than from intermediate data where the solution already has symptoms of divergence.