The final step for the development of a CFD simulation for a problem of interest is to process and examine the validity of the obtained numerical results (a.k.a post-processing and validation step). This steps requires an in-depth engineering knowledge about the fundamentals of the physical problem of interest. Thus, the value of investing time in understanding the fundamental physics of the flow, once again is highlighted here. This process is done starting from general inspection on CFD simulation results and ends with more detail validation process.
The first general rule of thumb to check the convergence of a CFD simulation is to visualize the residuals for key flow variables, such as continuity, momentum, velocity and etc.. In STAR-CCM+ once user starts to run the simulation, the Residual values for the relative variables, based on the choices of models, are visualized in the solver window. Furthermore, users can manage details of the plotted residuals or add other residuals to be visualized via Plots/Residuals.
Fig. 1 visualizes the residual values of continuity and momentum in x-direction versus the number of iterations. The general decreasing trend of the residual values confirm that the numerical solution of the conservation/governing equations are converging to specific final values. Usually the residual for the continuity decreases with the slower rate compared to other residual values. Therefore, a continuity residual of 10E-3, is the first necessary, but not sufficient, general criteria to confirm the convergence of the CFD simulation. In this case, this criteria is reached after about 250 iterations and after about 700 iterations the continuity residuals reached value of 5E-4, which is a solid confirmation of CFD simulation convergence.
Users can also define criteria to stop the iteration process once the desired criteria is during the iteration process to find flow field solution. These settings are available at via Stopping Criteria\ [right click] path. In the current case study two criteria was set to stop the simulations: 1- Reaching via Stopping Criteria\Maximum Steps of 800 OR 2- Reaching the Stopping Criteria\Continuity Criterion of 1E-6. For the case of Re=100 the latter criterion was reach first and iterations were stopped after 800 iterations as shown in Fig. 1.
The second step is to visualize dimensionless form of the important variables within the CFD domain. This visualization step can be problem specific and should be performed over an adequate plane of choice. For most of the problems contour of normalized velocity or pressure, over a horizontal or vertical plane at the center of the CFD domain, is a good start point. The path to define an adequate probe such as planes or lines is Derived Parts/ [right click]. With this path a user can define various type of probes to visualize the obtained numerical results over them. However, for the current problem since the entire domain is two dimensional and planar, it would make the entire domain the best candidate for the post-processing plane.
User should now define the normalized variable of interest that needs to be visualized. The normalized streamwise velocity by the inlet velocity can be defined using Tools/Field Functions/ [[right click], name the variable in Function Name (i.e. Ux/U0) and put the required formula for the variable of interest with correct syntax under Definition (i.e. $${Velocity}[0]/1). This will calculate the normalized streamwise velocity with free stream velocity within entire CFD domain. It order to visualize the defined normalized flow field variable in the previous step users should use Scenes/Scalar Scene 1/Displayers/Scalar 1/Scalar Field and choose the Ux/U0.
Fig. 2 visualizes the normalized streamwise velocity with free stream for four different flows with various Reynolds numbers (specified on each contour). The general physics for all four flows are the same. Flow enters the domain with normalized velocity of 1. Due to the imposed no slip boundary conditions on the flat plate, the velocity instantly decrease to zero at edge of the plate and the boundary layer starts to form and grows moving further downstream the plate. Furthermore, Fig. 2 visualizes that by increasing the order of magnitude for the Reynolds number, increasing the effect of inertial forces over viscous forces, the thickness of boundary layer along the flat plate decreases. This agrees with the general physics of this flow field, which states the local laminar boundary layer thickness (δ) is proportional to the inverse square root of local Reynolds number. It should also be highlighted that these velocity contours are smooth. The smoothness confirms the validity of created mesh resolution and convergence of the numerical solution. However, this is only an additional necessary, but not sufficient criteria for simulation validity and convergence.
After performing the general post-processing steps, the user need to perform more detail oriented post-processing to confirm the validity of the CFD simulation. This stage can be a state-of-the-art. Comparing the numerical results against the theory (discussed earlier) or any other available experimental results is the final stage of post-processing. It is extremely important to calculate the correct corresponding numerical variables and compare them against the experimental or other numerical data.
For the problem of two dimensional laminar flow over a flat plate, users can visualize the variation of normalized streamwise velocity with the free stream $\frac{U_x}{U_0}$ versus the similarity variable $\eta$. As discussed earlier in the physics section of this problem, if $\frac{U_x}{U_0}$ is plotted versus non-dimensional similarity variable $\eta$, instead of dimensional variables such as $U_x$ and $X$, it should shows a universal curve for any Reynolds number and any position along the plate. Fig 3 visualizes the variation of $\frac{U_x}{U_0}$ against $\eta$ for the Reynolds number of 10E+4 at all point's within the CFD domain. In order to visualize users should define the equation for the similarity variable $\eta$ in Tools/Field Functions as discussed earlier and add a new XY-Plot via Plots/ [right click] path. Setting the previously defined Field Functions to the corresponding axes will result in to the following figure:
Fig. 3 shows that the evolution of the velocity at any point with respect to the similarity variable is in a good agreement with the trend discussed in the physics section. The interesting observation here is that if users get the same plot for other case studies with lower Reynold numbers it will be observed that as the flow Reynolds number increases the plotted curve matches the expected experimental trend better. The reason behind this observation is that increase in Reynolds number order of magnitude lead to decrease of boundary layer thickness, which is one of the most fundamental assumption of Blasius solution. Therefore, the visualized trend for flow with Re=10E+4 shown in Fig. 3 is almost identical to the presented experimental results in physics section of this tutorial.
At this stage one can conclude that this CFD numerical simulation is validated to study laminar flow over a flat plate. For further validation one can visualize the variation of friction force/coefficient along the plate for different Reynolds number and compare the results against the corresponding theory. Therefore, it can be used for similar or more complex problems, such as flow with specified pressure gradient, non-uniform velocity profiles and etc.. This can be done via correct implementation in changing the corresponding boundary conditions.
In [ ]: