CFD Quiz

None, the Reynolds number is a dimensionless value​

Dynamic viscosity relates shearing stress to fluid motion and has the SI unit of Pa-s or the customary unit Centipoise (1cP = 0.001 Pa-s). The kinematic viscosity is the ratio of the dynamic viscosity to the density of the fluid, and has the SI unit of m²/s or the customary unit of Stokes (1^St = 1 cm²/s).

The density will stay the same as the volume is constant, and no mass is entering or leaving the enclosure. The pressure will increase with the higher temperatures​

The volume is proportional to temperature and will occupy a larger volume at a higher temperature, assuming the pressure remains the same. ​

The Nusselt number defines the ratio of total heat transfer at the boundary to the conductive heat transfer. With this ratio, you can define the heat transfer convective coefficient. This value was named after Ernst Kraft Wilhelm Nußelt. ​

SCFM stands for Standard Cubic Feet per Minute, while CFM is the actual flow rate running down the duct. In the US, standard conditions are typically assessed at 68°F and 1 atmosphere, while this reference may be different for other places in the world. The important part, is that from the standard values for pressure and temperature (which will be lower than the problem statement), you can deduce a mass flow rate. When working back through the ideal gas law for the operating conditions, you will realize a lower density than standard conditions, which will result in a much higher actual flow rate than 200 CFM, resulting in higher mean velocities for 200 SCFM. ​ ​

Laminar flow consists of smooth parallel streamlines of velocity without the presence of mixing, local eddies, or random velocity fluctuations. Within a pipe, laminar flow will result in a parabolic velocity profile from the walls, whereas fully developed turbulent flow will have a flatter mean average velocity profile near the center.

The fluid velocity vector from a RANS simulation will represent the time average or mean average of the velocity field. This value does not include instantaneous velocity fluctuations resulting from flow turbulence

Solution:

In most cases, choice B is the best combination of those listed, as it provides a combination of boundary conditions most compatible with the governing equations. Options C and D may also be good choices for particular conditions, but could lead to convergence issues in some cases. Option A should be avoided at all cost as it could lead to setup error issue, divergence, and provides no information on pressure, which is critical for state calculations.

Let’s look at this quick example below of compressed air flowing through a nozzle. Cases B through D work well for this option and all provide repeatable results on mass flow, pressure drop, and peak Mach number achieved through the orifice. Option A provides wildly different results on peak Mach number and pressure drop. This is due to the fact that none of the boundary conditions provide a reference for pressure, so the solution must rely on the initial pressure conditions to float to a converged solution.

No:

This is a classic trap in fluid mechanics and CFD, where the geometry defining the flow path is symmetric, but the end result will not be. Exterior flows over bluff bodies or cylinders will induce wake zones and recirculation regions. In addition, the flow will also separate from the body at sharp angles or on the downstream side. These vortices that develop will not completely balance one another, inducing a transient phenomena known as vortex shedding. This is not a numerical artifact of the CFD solution, but a real and observed effect that can cause structural damage through modal coupling.

The example below shows two cases of flow over a bluff body where we apply a symmetry boundary at the midplane (top), and where we model the full span (bottom). The symmetry boundary forces the recirculation zone to be balanced and stabilizes the point of flow separation. Although this looks nice and neat, this would not reflect reality. With a full span model, we can observe the vortices coming off the rear end of the body, which are not symmetric.

C will give you the most accurate model to capture potential secondary flow. Of the models listed, the Reynolds stress model is the only one to capture the anisotropic nature of turbulence and secondary flows. This model will add six additional equations to solve which will significantly increase computational effort and can lead to convergence challenges. You will need to ask yourself, just how important this additional level of detail is. In the example model below, the RKE model does not capture the well known secondary flow swirl that develops in rectangular ducts and underpredicts the pressure drop by more than 10%.

No. The Navier Stokes equations are only valid for continuum flow conditions. The low pressure conditions here require us to determine what flow regime we are in by evaluating the Knudsen number to determine flow rarefication. The Knudsen number is the ratio of the molecular mean free path, 𝜆, to the pertinent dimension, 𝐿, which is our gap dimension of 2.5 mm.

The molecular mean free path is the average distance traveled by a gas molecule between collisions and can be defined by the following relationship:

Where 𝜇 is the dynamic viscosity, 𝜌 is the gas density, 𝑅 ̅ is the universal gas constant, 𝑀 is the molecular mass, and 𝑇 is the gas temperature. From the Knudsen number, the various flow regimes are defined as follows:

Based on the defined temperature, pressure, and gap from the problem, we calculate a Knudsen number of 3.5, which puts us in the free molecular flow regime.

In the application used, Simcenter STAR-CCM+, the plotted working pressure is roughly equal to the static pressure (aside from a small turbulence effect and hydrostatic effects). Since there is no height change in the above problem, we can step back from CFD and look at the Bernoulli equation for flow down a streamline in the center of the pipe near the expansion (to ignore the pipe head-loss on either side):

As the water is incompressible, the volumetric flow rate is constant throughout, so the velocity decreases through the expansion with the larger cross-sectional area. With the velocity after the expansion, 𝑣₂, lower than the inlet, 𝑣₁, The static pressure at 𝑃₂ must be higher than 𝑃₁ to balance the relationship. This is the culprit of why we have an unintuitive increase in pressure in the direction of flow.

A better way to present this data is to use the Total Pressure. The total pressure will sum the static, dynamic and hydrostatic components. What will be left is the expected decrease in pressure with flow direction due to losses

NO. The All Y+ turbulence models in major commercial codes seek to bridge the gap between directly modelling the viscous sublayer, or using a logarithmic wall function, in the outer log-law region of the boundary layer. This Y+ value is a dimensionless number that is determined by the distance of the1st cell to the wall, frictional velocity, and kinematic viscosity (similar to a local Reynolds number). Y+ values less than 5 show the cell is in the viscous sublayer region next to the wall. Y+ values above 30 state a logarithmic wall function can be used to estimate the flow. In between these values is a no-mans land. This is a buffer layer where commercial codes implement a smoothing function to bridge these two regimes together. This allows CFD engineers to model complex flow through complex geometries where it would be nearly impossible to create a mesh that completely falls in either the viscous sublayer or log-law region. Having small areas that fall within the buffer layer using the All Y+ methods is sometimes unavoidable, but if a significant portion of the model is in this region, the results will be severely compromised.

To demonstrate the impact of what a poor mesh could have on your thermal results, we re-ran the study presented by Siemens in their support article comparing the impact of wall functions on thermal results, but we add in a third case with a poor choice for Y+. This is a simple case of flow down a tube with a constant wall temperature. We see the wall functions lead to a 1% to 2% over prediction of heat flux, which is a manageable difference. In comparison, the poor choice in Y+ leads to a significant error of under predicting the heat flux by 5% to 10%. For small regions within a model, this impact will be negligible on the final solution, but if these values represent a large portion of the model, delete the result and start over.

False. The CFL (or Courant number) is the ratio of analysis time step to the time it takes the fluid to travel across the width of the cell. For an explicit analysis, this value must be less than 1 for all cells (i.e. the fluid never fully transverses the cell during a time step). With implicit schemes, that utilized inner loop iterations to solve for a particular time step, these values can be greater than 1 to speed up the solution time. Average values of up to 5 or 10 can be achieved, but this still depends on the overall dynamics of the flow. For highly dynamic flow, we would suggest trying to keep the CFL value close to or below 1.

To demonstrate this capability, we performed a laminar vortex shedding analysis with different time steps, as seen in the video below. The timesteps result in maximum CFL values of 1, 2, and 6 respectively. This is a fairly dynamic problem, and we are able to get solutions for all time steps using the implicit solver. The larger time step with a CFL of 2 provides a pretty close comparison to the suggested solution method, but as we get the time step much larger, where the maximum CFL value is 6, we start to see a significant amount of numerical diffusion.