Physical Model Sensitivity

Setting up a CFD simulation requires the selection of a number of physical models. The purpose of the physical model is to mathematically represent the physics of a process that occurs in the simulation. One of the first steps in defining the simulation is the identification of the relevant physics that need to be modeled. Once this is done, a suitable model needs to be selected for each aspect of the simulation. Because various models exist for different characteristics of a simulation, it is important to investigate the sensitivity of the results to each of them. The following list mentions some of the possible physical models that need to be considered.

Flow Physics and Modeling

Flows can exhibit different physics under different conditions which must be carefully considered when setting up a simulation. A few variations of these are discussed below.

Steady and unsteady flows: In steady flows, flow properties, such as velocity and pressure, at a given point do not depend upon time.; In unsteady flows, flow properties at a point are functions of time.; Steady flow model is actually a simplification, and it is valid only when the time period over which the flow is observed is large. For modeling a steady flow, the time dependent terms in the Navier-Stokes governing equations are dropped.
Compressible and incompressible flows: Flows with Mach number up to 0.3 at room temperature are said to have weakly compressible behavior, and for the purpose of simulation can be considered incompressible flows, assuming the density to be constant.; Flows with Mach number greater than 0.3 are compressible where the fluid flow should account for the variation of fluid density.
Viscous and inviscid flows: Viscous flows are those in which frictional effects between fluid layers and fluid layers and surfaces are significant. All real flows are viscous flows.; Inviscid fluid flow model is a simplification that can be applied in cases when viscosity effects are expected to be small in comparison to inertial forces. High Reynolds number flows in large size domains where viscosity effects are limited to the small regions close to the boundaries can be considered as inviscid flows for bulk of the domain.
Single-phase and multi-phase flows: Single-phase flows are those in which the flow domain contains only one fluid material in a single state throughout the domain.; In case this condition is not satisfied the flow may be considered multiphase. Multiphase flows can contain a single material in different states or a mixture of two or more different materials in the same or different states. Examples of multiphase flows include solid or liquid particles immersed in a liquid medium or liquid droplets in gaseous medium.; Some common methods for dealing with multiphase flows are Volume of Fluid (VOF) method and Level Set method. Often the multiphase methods are not standalone methods to solve the complete flow field but track the interface between the existing phases.
Laminar and turbulent flows: Laminar flows are characterized by a highly ordered fluid flow where fluid flows in smooth non intersecting layers.; Turbulent flow is characterized by its irregular flow regime where fluid layers are not easily distinguished. Rapid changes are experienced in a turbulent flow regime. Instead of layers turbulent flows are made up of eddies of various sizes. These eddies constantly form and dissipate as they interact with each other in a rather chaotic manner.; The characterization between the laminar and turbulent nature of a flow is usually done on the basis of the Reynolds number (Re) for the flow. Pipe flows with Re < 2300 are laminar. Flows with Re > 4000 are considered turbulent. For flows with Re-value between these ranges the flow is said to be in a transition state.; If the problem is identified as a case of turbulent flow you must decide on the turbulence model to use for the problem. There are a number of choices available for this and not all models behave similarly in all situations. The following discussion is about making the choice of the turbulence model for the problem.

Turbulence Physics and Modeling

Turbulent flows have eddies of various scales. These eddies interact with each other causing rapid changes in flow properties. The highly chaotic nature of the flow makes modeling it a challenge.

The smallest turbulence eddies occurring in flows can have extremely small length scales. Direct simulation of these eddies requires mesh and temporal resolution which exceeds the computational capabilities of most modern computers. The computationally effective way is to model the behavior of the turbulent eddies in a time averaged flow field.

Turbulence models are used to predict the effects of turbulence in the fluid flow without resolving all of the small scales of motion that are associated with a turbulent flow. This reduces the amount of computing time necessary to obtain a solution to a fluid flow problem.

Most CFD solvers contain a broad selection of different turbulence models. The most commonly employed models in the industry are based on the Reynolds-averaged Navier-Stokes (RANS) equations. Among RANS models there are eddy viscosity and Reynolds Stress formulations that need to be considered. Alternative approaches such as Detached Eddy Simulation (DES), Large Eddy Simulation (LES) and Direct Numerical Simulation (DNS) are also available in many CFD solvers. DNS approach, as the name suggests, is the approach that directly solves for eddies of all scales and does not involve any kind of modeling. It is mostly employed only for research purposes. Accuracy and computational requirements for these approaches is as follows.

RANS < DES < LES < DNS

When setting up a simulation it is your responsibility to select a suitable turbulence model for your application. Many models provide a reasonable level of accuracy for a broad range of applications while others are formulated specifically for certain flows. Among the most popular general purpose models are the one equation Spalart-Allmaras (SA) model and the two equation Shear Stress Transport (SST), and k-omega (k – ω) models.

Even while using general purpose turbulence models the choice of the model is important with respect to the problem being analyzed. Some models are better suited to some flows than others. The accuracy of a given turbulence model is highly case dependent and there are no established rules that can ensure correctness of the chosen model for a specific application. You must always proceed with caution and choose a turbulence model only after verifying its suitability to previously benchmarked problems of a similar nature.

In addition to the selection of a turbulence model it is also important to consider whether the flow is fully turbulent or transitional. If the flow is transitional it is important to include a transition model to properly account for this effect.

Wall modeling for turbulent flows: The use of a wall model is common practice when simulating high Reynolds Number viscous flows. The wall model relaxes the near wall meshing requirement to resolve the turbulent boundary layer and results in a reduction in required overall mesh count. Most wall models are formulated for simple boundary layer flows with no adverse pressure gradient. The application of these wall functions to non equilibrium boundary layers may impact accuracy.

Material Physics and Modeling

Setting up material properties is an important aspect of setting up a CFD simulation. Typically, CFD allows two types of materials, solids and fluids. Gases and liquids are both classified as fluids.

Setting up a solid model requires specification of density, specific heat and conductivity.

It is not required for a CFD model to have a solid material in the domain. These should be added only as required when an interaction between the fluid and the solid is present. Of the properties mentioned the specific heat and the conductivity are required only when energy equation is being solved.

Setting up a fluid model requires specification of the following properties:

Density
Viscosity
Specific Heat
Conductivity
Viscoelastic properties, if fluid exhibits viscoelastic behavior
Diffusivity for mass diffusion problems
Porosity for porous materials

Of the properties mentioned above specific heat and the conductivity are required only when energy equation is being solved.

The material properties in a CFD simulation can be defined in a number of ways. The simplest definition is specifying the properties as a constant value. Once specified these constant values do not change during the simulation. For solids, the conductivity can also be specified as constant, but anisotropic. That is a different but constant conductivity in each normal direction.

For some cases, however, specifying a constant value of properties is not exactly representative of the actual material behavior. For example, for highly compressible flows specifying a constant density will lead to inaccurate results. For such flows it is prudent to use the ideal gas model for the fluid density, which uses the ideal gas law to calculate density at a given time step.

There are various options available to specify the different properties for the materials. You should choose the option that resembles the actual conditions as closely as possible. Some options are as follows:

Linear or polynomial dependent on another variable (typically pressure, temperature or species)
A user-defined function
Ideal gas law for modeling density for compressible flows
Boussinesq model for density in naturally convected flows in which small density variations encountered in such flows can be neglected in all but the buoyancy terms. This approach should not be used if large density variations are expected.

Heat Transfer Physics and Modeling

When temperature field variations are expected to have a significant impact on the flow properties, or the temperature distribution is of interest in the analysis, the energy equation must be included in the governing equations.

The heat transfer modes available are conduction, convection (natural and forced) and radiation.

For highly viscous flows viscous heating of the fluid must be taken into account. An example of flows where viscous heating can have a significant effect are the internal flows in microchannels.

For simulating processes where the fluid undergoes adiabatic compression compression heating of the fluid must be taken into account as well.

Prandtl number (Pr) is an important parameter when heat transfer within the boundary layer is being studied. Prandtl number can, in simple terms, be described as being proportional to the rate of growth of the velocity and thermal boundary layers. Smaller values of Pr indicate that thermal diffusion is more prominent than momentum diffusion. Thermal boundary layer grows faster than the velocity boundary layer.

When temperature effects are being studied and the flow is turbulent it is also critical to take into account the additional effect of turbulence on heat transfer properties. The turbulent Prandtl number is an important parameter in this case. Experiments show the average value to be 0.85 for most applications, but the actual value can vary between 0.7 and 0.9 depending on the specific problem.

If radiation effects are present in the problem you must choose the radiation parameters accordingly. In case of enclosure radiation view factor computation between the enclosure surfaces is critical. In case of external incident radiation, for example solar radiation, solar flux vector should be specified.

Chemistry Models

Selection of chemistry models can play a critical role in the results of simulations of combusting and reacting flows. When selecting a chemistry model you need to consider the rate of the chemical reaction in comparison to the times scales of other events in the flow. Some models are geared specifically towards turbulent flows where the turbulent time scale is much slower than the chemical reaction. Others are intended for the opposite scenario.

The Backward Facing Step Case

For the backward facing step case you will be solving the RANS equation, which includes terms for viscous effects. The flow field can be considered incompressible and single phase, as the Mach number is below 0.3 (it is actually about 0.13), and air is the only fluid present in the domain. The flow within the domain is turbulent, as the inlet Reynolds number is 36000. The flow can be solved for a steady state solution as the inlet conditions or the fluid properties are not time varying.

In the solver setups used in previous sections the backward facing step case was solved using the SA turbulence model. To illustrate the sensitivity of the solution to the selection of turbulence model, the results from two models, the one equation SA model and the two-equation SST turbulence model, are shown in the table below. For this application, experimental data shows a reattachment length of 6.26 m. The results show that the SST model has a lower deviation from the experimental observation indicating that it is more suitable for this flow than the SA model.

Table 1. Turbulence Model Sensitivity for Backward Facing Step Simulation
Turbulence model	Reattachment length (m)	Percent difference from experiment
SA	5.96	4.8 percent
SST	6.40	2.2 percent