In order to keep the solution stable under extreme conditions, Ansys Fluent provides limits that keep the solution within an acceptable range. You can control these limits with the Solution Limits Dialog Box (Figure 36.13: The Solution Limits Dialog Box).
Solution → Controls 
Limits...
Fluent applies limiting values for pressure, static temperature, and turbulence quantities. Fluent also applies a minimum volume fraction for the matrix solution in Eulerian multiphase simulations run on a double-precision solver. The purpose of these limits is to keep the absolute pressure or static temperature from becoming zero, negative, or excessively large during the calculation, and to keep the turbulence quantities from becoming excessive. The purpose of the minimum volume fraction is to avoid singularity of the solution matrix when the volume fraction tends to zero.
Typically, you will not need to change the default solution limits. If pressure, temperature, or turbulence quantities are being reset to the limiting value repeatedly (as indicated by the appropriate warning messages in the console), you should check the dimensions, boundary conditions, and properties to be sure that the problem is set up correctly and try to determine why the variable in question is getting so close to zero or so large. You can create a field variable cell register to mark and display cells have a value equal to the limit (refer to Field Variable for more information). In very rare cases, you may need to change the solution limits, but only do so if you are sure that you understand the reason for the solver’s unusual behavior. For example, you may know that the temperature in your domain will exceed 5000 K. Be sure that any temperature-dependent properties are appropriately defined for high temperatures if you increase the maximum temperature limit. Another rare example is when the actual volume fraction in the domain needs to go below a safe limit of 1e-08, such as in nucleation and dispersion of very low amounts of contaminants in a system. By reducing this limit you may encounter instability problems.
Important: The absolute pressure limit is enforced only for fluid materials that are modeled using the ideal-gas or one of the real-gas-* density methods.
For materials that use the compressible-liquid or a user-defined compressible fluid (liquid or gas) density method, a pressure limit is used to ensure that the density remains positive, but the actual pressure value itself is not limited.
Note that if you are using the density-based solver and the temperature and/or pressure values are approaching the minimum and/or maximum limits, you can enable divergence prevention to apply under-relaxation to the variables in select cells rather than changing the limits. For details, see Preventing Divergence Using Local Under-Relaxation.
For additional information, see the following sections:
The limiting minimum and maximum values for absolute pressure are shown in the Minimum and Maximum Absolute Pressure fields. If the Ansys Fluent calculation predicts a value less than the Minimum Absolute Pressure or greater than the Maximum Absolute Pressure, the corresponding limiting value will be used instead. Similarly, the Minimum and Maximum Temperature are limiting values for energy calculations.
The Minimum Turb. Kinetic Energy, Minimum Turb. Dissipation Rate, and the
Maximum Turb. Viscosity Ratio are limiting values for turbulent calculations. If the calculation predicts a value
for 
or 
that is less than the appropriate limiting value (that is, Minimum Turb. Kinetic Energy or
Minimum Turb. Dissipation Rate, respectively), then the limiting value will be used instead. For the viscosity
ratio limit, Ansys Fluent uses the limiting maximum value of turbulent viscosity (
) in the flow field relative to the laminar viscosity. If the ratio calculated by Ansys Fluent exceeds the limiting
value, the ratio is set to the limiting value by limiting 
to the necessary value.
For Eulerian and Mixture multiphase simulations run on a double-precision solver using the implicit volume fraction formulation, if the prediction of volume fraction falls below the value specified for Minimum Vol. Frac. for Matrix Solution, Ansys Fluent will use the limiting value in the matrix solution for phase-specific equations, depending on the model.
For the multiphase models supporting the explicit volume fraction formulation and for the VOF model, the Volume Fraction Cutoff limit specified in the Multiphase Model dialog box will serve as a limiting value when solving phase-specific equations, depending on the model.
Note: The Eulerian multiphase model uses the specified solution limits for solving Momentum, Turbulence, Energy, Species, and UDS equations, whereas the VOF and Mixture multiphase models use the specified limits for solving Species and UDS equations.
In Ansys Fluent’s density-based solver, the rate of reduction of temperature is controlled by the Positivity Rate Limit. The default value of 0.2, for example, means that temperature is not allowed to decrease by more than 20% of its previous value from one iteration to the next. If the temperature change exceeds this limit, the time step in that cell is reduced to bring the change back into range and a “time step reduced” warning is printed. (This reduced time step will be used for the solution of all variables in the cell, not just for temperature.) Rapid reduction of temperature is an indication that the temperature may become negative. Repeated “time step reduced” warnings should alert you that something is wrong in your problem setup. (If the warning messages stop appearing, the calculation may have “recovered” from the time-step reduction.)
Important: For high-speed flow, if your solution is diverging particularly for the energy equation, then lowering this limit to 0.05 or 0.02 might help in overcoming divergence.
When High-Speed Numerics (as described in Enabling High-Speed Numerics) is enabled, the positivity rate limit is also applied to the pressure update to ensure that the absolute pressure does not decrease by more than the prescribed positivity rate of reduction. A separate warning message for pressure indicating the number of limited cells is also printed.
If you change and save the value of one of the solution limits, but you then want to return to the default limits set by Ansys Fluent, you can reopen the Solution Limits Dialog Box and click the button. Ansys Fluent will change the values to the defaults and the button will become the button. To get your values back again, you can click the button.