Introduction to CFD Modeling Guidelines

The field of computational field dynamics (CFD) has seen tremendous advancement in recent decades, riding on the back of the phenomenal advances in computational science and power.

CFD evolved throughout the 20th century. In the pre-1950s, semi-analytical methods were developed to solve the complex problems that were still unsolved using analytical solution methods. During the same time period, numerical methods also advanced and became more mature with respect to numerical stability, speed and accuracy. Post 1950, with the availability of low cost computing power and advancement in computer science, researchers all over the world were able to develop complex CFD models and test them on a variety of applications, enabling the advancement of CFD at an accelerated scale. High-fidelity CFD solvers running on powerful computers today can accurately model complex fluid flows, solving the governing equations over billions of grid points, performing trillions of calculations at speeds unthinkable of a few years ago.

However, access to large amounts of computing power does not necessarily equate to high quality results from a CFD analysis. Modern CFD solvers are specialized and complex computer programs. The accuracy of the results provided by the solvers is subject to the accuracy of the inputs. It is necessary that a complete and correct set of inputs be provided to the solvers so that they can perform their task as correctly as possible. Some of the essential aspects of these inputs to be provided to the solvers are discussed in this section. You will be able to apply the basic yet important CFD analysis guidelines that are discussed to your own applications. Following these guidelines in most cases will ensure that the results obtained from the CFD analyses are reasonably accurate with only a small margin of error. However, it cannot be stressed enough that these guidelines should be treated as such, only guidelines, and not an authoritative set of instructions that will ensure correct analyses every time and for every application. You are both encouraged and solicited to apply sound engineering judgement to individual cases, as well as explore validation of your modeling methodology for each application of interest.

A CFD simulation involves solving of the complex Navier-Stokes equations, often coupled with other equations to determine distribution of flow, temperature and turbulence fields across a discretized simulation domain. The Navier-Stokes equations are highly nonlinear and are impossible to solve analytically with available methods. CFD solvers solve these equations numerically, often with a set of assumptions to simplify the solution and a set of parameters specific to the numerical method employed, to produce a stable solution. The numerical approach employed can vary from solver to solver. Also critical to the solution method is the set of constraints that you provide to the solver. This requires sound understanding of the problem definition and the objective of the simulation. At best, a CFD solver is a tool to simplify the task of solving the complex flow-field equations and must be applied carefully for the results to be a true and reliable representation of the actual physical processes. However, since even the best solver technique is based on a numerical approximation method, every CFD result has a degree of error and uncertainty introduced in it by these approximations.

Obtaining accurate results from a CFD simulation depends on many factors, such as how well you have modeled the conditions of interest and how well the CFD software has solved the equations necessary to model these conditions. In order to minimize the errors associated with a solution you must understand what these errors are. Some of these common error sources are listed below.
  • Modeling error: This type of error occurs because of the difference between the true physical processes and the equations that are used to model the processes.
  • Numerical or Discretization error: This type of error is induced because the model equations are not solved continuously but on a finite number of grid points in the domain.
  • Iteration or Convergence error: This type of error is induced because the solution is iterated to a finite convergence level, which is not zero.
  • Round-off error: This type of error is induced because the numbers are rounded off when stored in computer memory because of storage limitations.
  • Input errors: These are the errors induced due to uncertainties in inputs, such as the choice of physical model pertinent to the application, boundary condition specification and inaccurate input.
  • Code errors: These are the errors in the CFD solver code.
Ensuring accurate results requires extensive verification of the software and extensive validation of the modeling approach for the application of interest. Verification and validation are important to minimize the solver-side sources of error and uncertainty in the CFD analysis. Verification will ensure that the solver solves the equations correctly and validation tests the extent to which a chosen model accurately represents reality. Verification and validation are an important aspect of the CFD modeling process but will not be the focus of this discussion. Instead, this section focuses on general CFD quality assurance guidelines that you should follow to ensure that you can expect reasonable results from your analysis. The discussion is divided into several topic areas that represents an important aspect of modeling that addresses one of the error types discussed above. You need to be focused on these aspects, besides the user errors, to ensure high quality results. The following modeling aspects are discussed.
  • Geometric sensitivity for geometric uncertainties
  • Mesh sensitivity for discretization error
  • Boundary condition sensitivity for errors in boundary conditions input
  • Physical model sensitivity for modeling error
  • Convergence tolerance sensitivity for convergence error

For many CFD applications the true solution to the equations is not always known. In the absence of an analytical solution, or high quality experimental data to compare against, it is difficult to judge the accuracy of a CFD simulation. However, you can still investigate the suitability of your modeling practices by performing sensitivity studies. This practice reveals aspects of your model that have a significant impact on your solution. Once these aspects are identified further work can be done to determine the most appropriate modeling practices for each of these aspects that will minimize the error associated with the individual aspects, ensuring good quality of results overall. It should be noted that performing a full suite of sensitivity studies to evaluate the solution is a costly and time consuming process. Since there are a number of aspects to be evaluated and all of them can impact the solution combining all of them in a single study is not advisable. It is best to study them one at a time. When performing a sensitivity study one aspect of the model that is being studied should alone be changed and everything else should be kept unchanged until a satisfactory solution is achieved. This process is then repeated for all of the aspects that you are interested in studying. In practice, many investigations are avoided and engineering judgment is used in its place. However, for applications where accuracy is of high importance a full set of sensitivity studies needs to be performed to ensure that modeling errors are minimized in the solution. It should be remembered that the sensitivity studies cannot take into account user and code errors and do not warrant that the solution achieved will be the true physical solution. The following discussion describes different sensitivity studies that are commonly performed when investigating the modeling practices to produce a quality solution.

As an exercise, and also to demonstrate to you the effect of the choices made for each of these aspects over the course of a sensitivity study, the discussion of the topics covered will be accompanied with the discussion of a simple but interesting case, the backward facing step case. For a detailed description of the case refer to the AcuSolve Validation manual in your AcuSolve installation directory. However, here you will not analyze the case with the objective of validating the model but with emphasis on educating you about guidelines for setting up the model correctly and identifying the appropriate modeling choices to make. A brief discussion of the case is as follows.

The problem consists of a fluid flowing in a channel with a sharp expansion. The step in the channel causes the flow to detach at the step and reattach some distance downstream of the step. The detached flow also causes recirculation in the region between the step and the reattachment point. The fluid properties are close to that of air. The Reynolds number at the inlet is 36,000, which is based on the step height. The flow is turbulent and you will pursue a steady state solution. The objective of the analysis is the accurate representation of the recirculation zone and determination of the reattachment point. The image below shows the schematic geometry of the case setup.
Figure 1. Schematic Geometry of the Backward Facing Step Case

This situation roughly mimics the behavior of flow exiting from a flow channel into a plenum of a plate type heat exchanger. An engineer is interested in placing a pressure tap along the lower wall to measure the total pressure drop through the system. In order to avoid spurious measurements from the pressure tap it is necessary to place the tap downstream of the recirculation region. Therefore, the location of the reattachment point must be known.