Tags

- ANSYS
- ANSYS CFX
- ANSYS Fluent
- CD-Adapco
- CD-Adapco StarCCM+
- cfd
- CFD engineer
- Computational
- computational fluid dynamics
- epsilon
- Fluid Dynamics
- Fluid Mechanics
- k-epsilon
- k-omega
- law of the wall
- mesh generation
- Navier Stokes
- omega
- OpenFoam
- StarCCM+
- turbulence
- turbulence intensity
- turbulent viscosity ratio
- viscosity ratio
- wall damping function
- wall function

Just how much k turbulence do you need entering your simulation? Turbulence demands modeling just like any other equation in computational fluid dynamics (CFD). As the CFD engineer, you need to describe boundary conditions for your turbulence equations. For a typical k-omega turbulence model, what are the appropriate values for k and omega as boundary conditions? This article discusses modeling boundary conditions for turbulence.

Most turbulence models utilize two-equation models; this in turn requires two boundary conditions at the inlets and outlets of our CFD model. We normally don’t directly specify values for the turbulence model. Instead, we deal in two more comprehensible terms:

- Turbulent viscosity ratio
- Turbulence intensity

After specification, these get converted into the actual terms required for the individual turbulence model.

The first boundary condition comes from the turbulent viscosity ratio. This was the ratio of the turbulent viscosity to the actual physical viscosity of the fluid.

- R
_{T}= μ_{T}/ μ

The best resource for typical values is the NASA Turbulence Modeling Resource [1] Based on that, and other CFD experience, Table 2‑1 supplies general guidance for typical turbulent viscosity ratios.

**Table 2‑1: Typical Turbulence Ratios**

R_{T} = 1 | Low |

R_{T} = 10 | Medium |

R_{T} = 100 | High |

R_{T} = 1000 | Very high (Unlikely, but tolerable in simulation) |

R_{T} = 10,000 | Not physically possible on Earth |

As a default setting, most CFD engineers go with a viscosity ratio of 10; it provides a nice medium level of turbulence.

When troubleshooting your simulation, plotting the viscosity ratio can be helpful. A viscosity ratio of 1000 or greater should not generally exist in the domain. These normally indicate problems with low resolution in your mesh. You may choose to tolerate high viscosity ratios at small isolated sections of the mesh, if these sections are in non-critical regions of the fluid domain. But understand that they still indicate problems with the mesh and potential instability.

The second boundary condition comes from turbulence intensity. In the classic RANS definition, we separate the velocity into the steady component and the fluctuating turbulent component. Turbulence intensity takes the ratio of these two components, normally expressed as a percentage.

Table 3‑1 shows typical values for turbulence intensity. Most CFD engineers take 5% as a good default value. Normally, you want to match the turbulence intensity to the viscosity ratio. Don’t select a high viscosity ratio and match that to a low turbulence intensity. The only exception would be if you had experimental data proving it was more appropriate.

**Table 3‑1: Typical Values for Turbulence Intensity**

1% | Low |

5% | Medium |

10% | High |

Wall boundary conditions require special consideration for turbulence. Remember the law of the wall; all turbulent boundary layers have a laminar sub-layer. The CFD software knows this, and the CFD developers generally approach this with two possible solutions:

- Wall damping functions
- Wall functions

A wall damping function assumes you defined a very fine mesh that resolved the entire boundary layer, with cells going all the way down into the laminar sub-layer. In this case, the damping function reduces turbulence near the wall, based on the Y+ distance.

Alternatively, a wall function assumes the entire laminar sub-layer was contained within the thickness of the first cell on the wall. Rather than damping out the turbulence model, it integrates the effect of the laminar sub-layer and applies that effect within that first cell only. All the cells remain fully turbulent.

The meshing strategy for the CFD engineer depends on the selected wall function. The mesh height near the wall must be set to match the selected wall treatment. And we measure mesh height by Y+. Y+ is a non-dimensional measure of the distance from the wall, and practically every CFD solver can calculate this value. Table 4‑1 shows recommended values for Y+ settings. The table shows the Y+ value for the typical break between laminar sub-layer and turbulent boundary layer. But most CFD engineers prefer to include a safety margin and ensure their entire body remains meshed with the correct settings. The third column in the table shows recommended settings with those safety margins.

**Table 4‑1: Recommended Values for Y+ Ranges**

| Y+ Range | Recommended Setting (with safety margin) |

Wall damping function | 12-30 | 2-5 |

Wall function | 30+ | 40 – 80 |

Don’t let the complexity of turbulence intimidate you. It remains subject to the same limits of transport equations, just like any other. It requires boundary conditions just like the rest. Thankfully, we have ample modeling resources to work with and comprehensible terminology for boundary conditions. Turbulent viscosity ratio and turbulence intensity form the basis for defining our turbulent boundary conditions. These two values can be used to calculate the actual equation quantities for most turbulence models and specify inlet and outlet boundary conditions. After that, the CFD engineer needs to ensure that their mesh matches the model settings at the wall boundary conditions. That completes the settings to successfully bound the problem of turbulence.

[1] | Langley Research Center, “Turbulence Modeling Resource,” National Aeronautical and Space and Administration, 03 Feb 2019. . Available: https://turbmodels.larc.nasa.gov/index.html. . |

[2] | TCFD, “Axial Compressor CFD,” TCFD, 31 Dec 2018. . Available: https://www.cfdsupport.com/axial-compressor-cfd-simulation.html. . |

[3] | Atsushi Ueyama, “Progress of Time,” Cradle MSC Software Company, 31 Dec 2018. . Available: https://www.cradle-cfd.com/tec/column01/017.html. . |

[4] | YouTube Author: Holzmann CFD, “Holzmann CFD & OpenFOAM® – Dynamic Meshes in Multiphase Flows #2 (Topology Change, Ship Simulation),” YouTube, 10 Feb 2018. . Available: https://www.youtube.com/watch?v=B9KjnyDpsx0. . |