CFD Online Logo CFD Online URL
Home > Forums

Convergence in ANSYS Fluent

Register Blogs Members List Search Today's Posts Mark Forums Read

Rating: 2 votes, 4.50 average.

Convergence in ANSYS Fluent

Posted December 13, 2013 at 06:00 by Centurion2011

At convergence, the following should be satisfied:
  • All discrete conservation equations (momentum, energy, etc.) are obeyed in all cells to a specified tolerance OR the solution no longer changes with subsequent iterations.
  • Overall mass, momentum, energy, and scalar balances are achieved.
  • Monitoring convergence using residual history:
  • Generally, a decrease in residuals by three orders of magnitude indicates at least qualitative convergence. At this point, the major flow features should be established.
  • Scaled energy residual should decrease to 10-6 (for the pressure-based solver).
  • Scaled species residual may need to decrease to 10-5 to achieve species balance.
  • Monitoring quantitative convergence:
  • Monitor other relevant key variables/physical quantities for a confirmation.
  • Ensure that overall mass/heat/species conservation is satisfied.

In addition to residuals, you can also monitor lift, drag and moment coefficients.

Relevant variables or functions (e.g. surface integrals) at a boundary or any defined surface.

In addition to monitoring residual and variable histories, you should also check for overall heat and mass balances.

The net flux imbalance (shown in the GUI as Net Results) should be less than 1% of the smallest flux through the domain boundary

If solution monitors indicate that the solution is converged, but the solution is still changing or has a large mass/heat imbalance, this clearly indicates the solution is not yet converged.

In this case, you need to:
  • Reduce values of Convergence Criterion or disable Check Convergence in the Residual Monitors panel.
  • Continue iterations until the solution converges.

Selecting None under Convergence Criterion disables convergence checking for all equations.

Numerical instabilities can arise with an ill-posed problem, poor-quality mesh and/or inappropriate solver settings.
  • Exhibited as increasing (diverging) or “stuck” residuals.
  • Diverging residuals imply increasing imbalance in conservation equations.
  • Unconverged results are very misleading!

  • Ensure that the problem is well-posed.
  • Compute an initial solution using a first-order discretization scheme.
  • For the pressure-based solver, decrease underrelaxation factors for equations having convergence problems.
  • For the density-based solver, reduce the Courant number.
  • Remesh or refine cells which have large aspect ratio or large skewness.
  • Remember that you cannot improve cell skewness by using mesh adaption!

Under-relaxation factor, α, is included to stabilize the iterative process for the pressure-based solver
  • Use default under-relaxation factors to start a calculation.

Decreasing under-relaxation for momentum often aids convergence.
Default settings are suitable for a wide range of problems, you can reduce the values when necessary.
Appropriate settings are best learned from experience!

For the density-based solver, under-relaxation factors for equations outside the coupled set are modified as in the pressure-based solver.

A transient term is included in the density-based solver even for steady state problems.
The Courant number defines the time step size.
For density-based explicit solver:
  • Stability constraints impose a maximum limit on the Courant number.
  • Cannot be greater than 2(default value is 1).

Reduce the Courant number when having difficulty converging.
For density-based implicit solver:
  • The Courant number is not limited by stability constraints.
  • Default value is 5.

Convergence can be accelerated by:
  • Supplying better initial conditions
  • Starting from a previous solution (using file/interpolation when necessary)
  • Gradually increasing under-relaxation factors or Courant number
  • Excessively high values can lead to solution instability convergence problems
  • You should always save case and data files before continuing iterations
  • Controlling MultiGrid solver settings (not generally recommended)
  • Default settings provide a robust Multigrid setup and typically do not need to be changed.

A converged solution is not necessarily a correct one!
  • Always inspect and evaluate the solution by using available data, physical principles and so on.
  • Use the second-order upwind discretization scheme for final results.
  • Ensure that solution is grid-independent:
  • Use adaption to modify the grid or create additional meshes for the grid-independence study

If flow features do not seem reasonable:
  • Reconsider physical models and boundary conditions
  • Examine mesh quality and possibly remesh the problem
  • Reconsider the choice of the boundaries’ location (or the domain): inadequate choice of domain (especially the outlet boundary) can significantly impact solution accuracy

Numerical errors are associated with calculation of cell gradients and cell face interpolations.

Ways to contain the numerical errors:
  • Use higher-order discretization schemes (second-order upwind, MUSCL)
  • Attempt to align grid with the flow to minimize the “false diffusion”
  • Refine the mesh
  • Sufficient mesh density is necessary to resolve salient features of flow
  • Interpolation errors decrease with decreasing cell size
  • Minimize variations in cell size in non-uniform meshes
  • Truncation error is minimized in a uniform mesh
  • FLUENT provides capability to adapt mesh based on cell size variation
  • Minimize cell skewness and aspect ratio
  • In general, avoid aspect ratios higher than 5:1 (but higher ratios are allowed in boundary layers)
  • Optimal quad/hex cells have bounded angles of 90 degrees
  • Optimal tri/tet cells are equilateral

A grid-independent solution exists when the solution does not change when the mesh is refined.
Below is a systematic procedure for obtaining a grid-independent solution:
  • Generate a new, finer mesh.
  • Return to the meshing application and manually adjust the mesh.
  • OR Use the solution-based adaption capability in FLUENT.
  • VERY IMPORTANT: Save the case and data files first.
  • Create adaption register(s) and adapt the mesh. Data from the original mesh is interpolated onto the finer mesh. FLUENT offers dynamic mesh adaption which automatically changes the mesh according to user-defined criteria.
  • Continue calculations until convergence.
  • Compare the results obtained on the different meshes.
  • Repeat the procedure if necessary.

To use a different mesh on a single problem, use the TUI commands file/write-bc and file/read-bc to facilitate the setup of a new problem.
Better initialization can be obtained via interpolation from existing case/data by using solution data interpolation
A web-based training module is available to train users in replication of case setup and solution data interpolation.


Solution procedure for both the pressure-based and density-based solvers is identical.
  • Calculate until you get a converged solution
  • Obtain a second-order solution (recommended)
  • Refine the mesh and recalculate until a 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.
Posted in Uncategorized
Views 4333 Comments 0 Edit Tags Email Blog Entry
« Prev     Main     Next »
Total Comments 0



All times are GMT -4. The time now is 10:26.