### 15.10.5. Problems with Convergence

This section describes how to solve two general classes of convergence problems:

- Start-up Problems
- Later Problems

#### 15.10.5.1. Start-up Problems

If you are having problems getting your solution started, it will often be due to a poor initial guess. For details, see the following:

- Initialization Advice

- Recommended Configurations of Boundary Conditions

For some cases, in particular for compressible flow cases, you will need to first solve the case using simpler and more robust models and then use this solution as the initial guess for the more complex simulation. Below is a list of simulation attributes:

- Liquids and constant property materials are more robust than gases (in other words, incompressible flow is more robust than compressible flow).

- Laminar flow is more robust than turbulent flow with the Zero Equation Model, which in turn is more robust than the and other two-equation turbulence models, which in turn are more robust than Reynolds stress models. The zero equation model should not be used to obtain final results.

- Pressure specified Openings may be more robust than Static Pressure Outlets.

- The 1st Order advection scheme or a Specified Blend = 0 is more robust than the High Resolution scheme, which is more robust than a Specified Blend = 1. Smaller values of the Blend Factor are more robust than larger ones. Final results should use a Specified Blend of at least 0.75 or the High Resolution scheme. It is also possible that using a Blend Factor of 1.0 will not produce a converged solution no matter what you do. In this case, gradually increasing values of the Blend Factor could be used to get a more accurate solution than the 1st order option. If the flow includes shocks, the High Resolution scheme should be used.

- For transonic and supersonic flows, the most difficult flow regime is around Mach 1. If this is your flow regime of interest, you should first try a flow velocity lower or higher than Mach 1 and see how that converges. If this is successful, you can then modify your problem specification to your requirements and use the previous result as your initial value field.

- Smaller physical timesteps are more robust than larger ones.

- An Isothermal simulation is more robust than modeling heat transfer. The Thermal Energy model is more robust than the Total Energy Model.

- Velocity or mass specified boundary conditions are more robust than pressure specified boundary conditions. A Static pressure boundary is more robust than a total pressure boundary.

#### 15.10.5.2. Later Problems

If you have problems with convergence, you should find the source of the problem rather than taking the results as they are. There are many factors that may lead to poor convergence, including poor mesh quality, improper boundary condition selection and timestep selection to name a few. If you are unable to diagnose the source of your convergence difficulties, contact your technical support representative for advice.

When you are having problems converging, try to determine whether the problem is local or global. Compare the RMS and MAX residuals of the equations having difficulty. If the MAX residual is more than one order of magnitude larger than your RMS residual, it usually indicates that the problem is concentrated to a local region.

If it is a locally high residual, identifying the location of the MAX residual will help in diagnosing the problem. Typically the location of the MAX residual of the momentum equations is the most useful to identify. This may be done by reading the location of the MAX residual from the solver summary at the end of your OUT file, or by setting the Expert Parameter output eq residuals = true. For details, see CFX-Solver Expert Control Parameters.

If the MAX residual is far downstream of your region of interest and far from an outlet boundary, you may determine that it has no effect on your solution. If you write the equation residuals out to your RES file, then it may be useful to create an isovolume equal to your MAX residual criteria and to verify the residuals are low enough in your region of interest.

Once you have determined the location of your high residuals, you will want to determine the source of the local problem and fix it. Because CFD simulations are varied, a comprehensive list is not possible, but the following short list of common problems and solutions should be helpful. If you still cannot resolve your problem, contact your ANSYS CFX technical support representative for advice.

Table 15.1: Convergence Problems Due to Local Effects

Local Problem | Description and Solution
--- | ---
Poor grid quality | Small angles or high aspect ratios can lead to round-off errors in the solver. Try to improve grid quality in the problem area.

Free shear layer or wake

These often cause the convergence to stall due to transient effects. In most cases, the transients should be captured by the turbulence model and reflected as a mean velocity and turbulence intensity. A small timestep will resolve the transients, therefore causing the convergence problems. A larger timestep should take care of the problem. In some situations, it may also help to apply additional under-relaxation to the advection scheme gradients and blend factors. This can be done by adding the following text to the `ADVECTION SCHEME` CCL:

    ADVECTION SCHEME:
    Option = High Resolution
    Gradient Relaxation = 0.1
    Blend Factor Relaxation = 0.1
    END

`Blend Factor Relaxation` is applicable only for the high resolution scheme, while `Gradient Relaxation` is applicable for both the specified blend and the high resolution schemes. The default values of these parameters are 0.25 for steady-state simulations and 0.5 for transient simulations

MAX residual adjacent to a shock | The solution field can “bounce around” near discontinuities like shocks. Shocks can also be susceptible to a transverse instability called the carbuncle effect, particularly if the mesh is finer in the transverse direction than the flow direction. To resolve these issues, activate High Speed Numerics on the Advanced panel of the Solver Control tab.
MAX residual adjacent to a Stage Domain Interface | A large timestep can cause convergence problems at a Stage Interface. Reduce your timestep by a factor of 2 to 10. For closely coupled components, the Constant Total Pressure option should be considered. Increasing the pressure profile decay above its default of 0.05 may help robustness by adding stiffness to the downstream pressure profile, but can also reduce the natural circumferential pressure variation.
MAX residual adjacent to a flow boundary | Check that the boundary condition is sensible. Try different options for the boundary specification. If you can specify a profile (by equation or data interpolation), it may help. If you are using a profile, check to see that it is correct and sensible.

Table 15.2: Convergence Problems Due to Global Effects

Global Problem | Description and Solution
--- | ---

Large time scale effect

If the characteristic time scale is not simply the advection time of the problem, there may be transient effects holding up convergence. Heat transfer or combustion processes may take a long time to convect through the domain or settle out. There may also be vortices caused by the initial guess, which take longer to move through the entire solution domain.

In these cases, a larger timestep may be needed to push things through initially, followed by a smaller timestep to ensure convergence on the small time scale physics. If the large timestep results in solver instability, then a small time scale should be used and more iterations may be required.

Turbulence levels | Sometimes the levels of turbulence in the domain can affect convergence. If the level of turbulence is non-physically too low, then the flow might be “too thin” and transient flow effects may be dominating. Conversely if the level of turbulence is non-physically too high then the flow might be “too thick” and cause unrealistic pressure changes in the domain. It is wise to look at the Eddy Viscosity and compare it to the dynamic (molecular) viscosity. Typically the Eddy Viscosity is of the order of 1000 times the dynamic viscosity, for a fully turbulent flow.
Turbulence model selection | When choosing a turbulence model, care must be taken to use a mesh appropriate for the given model. Running a given turbulence model on an inappropriate mesh can cause convergence to stall.
Advection scheme | The 2nd Order High Resolution advection scheme has the desirable property of giving 2nd order accurate gradient resolution while keeping solution variables physically bounded. However, may cause convergence problems for some cases due to the nonlinearity of the Beta value. If you are running High Res and are having convergence difficulty, try reducing your timestep. If you still have problems converging, try switching to a Specified Blend Factor of 0.75 and gradually increasing the Blend Factor to as close to 1.0 as possible.

Release 18.2 - © ANSYS, Inc. All rights reserved.