In this article, we have discussed y+, a quantity used to describe fluid velocity near the walls. One way to characterize the velocity close to the walls is by using wall functions, whose equations are described below. This comparison of the functions with experimental results has been conducted in this article, and the wall function results demonstrate good accuracy. After describing the characteristics of the area near the wall and its simulation methods, the capabilities of ANSYS Fluent in simulating this important area have been described.

Contents

Toggle** **

## What is y+ in CFD?

If the fluid flow regime is turbulent, that means the ratio of inertial force to viscous force is very high. However, even in turbulent flows, near solid boundaries or walls the velocity decreases due to the no-slip condition. no slip condition means that the velocity of the fluid on the solid surface is zero, this assumption is not true everywhere, but it is true in many problems of fluid mechanics. This reduction in velocity leads to a decrease in inertial forces.

Consequently, the viscous force is relatively more effective and dominant in this region near the wall. This phenomenon creates a thin layer adjacent to the wall, known as the boundary layer, where viscous effects dominate and play a crucial role in determining the flow characteristics. Studying and understanding this area close to the wall is necessary for accurate simulation of fluid flow in that area and development of turbulence models.

Click to access the CFD Fluid Mechanics

## What is y+ in CFD Formula?

To describe the fluid flow near walls, two dimensionless quantities, u+ and y+, are used. These are defined as follows:

This equation is called **the law of the wall**. *U* is the velocity [m/s] at distance *y* from wall [y], *u _{t} *is the friction velocity [m/s],

*ρ*is the density [kg/m

^{3}], and

*μ*is the viscosity [Pa.s].

*τ _{w}* is the wall shear stress [Pa]. Generally, different y+ ranges are used for different purposes:

**Linear or viscous sub-layer (y+ < 5):** In this region very close to the wall, the fluid velocity is very low and the viscous force is completely dominant. That is why it is called the viscous sub-layer. It is assumed that the shear stress is approximately constant and equal to the wall shear stress. Thus:

After integrating with respect to *y* and applying the boundary condition *U*=0 when *y*=0, we obtain a linear relationship between the mean velocity and the distance from the wall.

By performing some algebraic operations and using the definitions of *u*+ and *y*+, we obtain:

Because of the linear relationship between *u*+ and *y*+, this area is known as the linear sub-layer.

**Buffer layer** **(5 < y+ < 30):** This layer is between the layers of the viscous sub-layer, where the viscous force is dominant, and the log-law layer, where the inertial force is dominant. In this layer, neither the inertia force nor the viscous force is dominant and both are effective. Therefore, the speed distribution in this layer is different from the previous and next layers

CFD simulation software addresses the buffer layer by utilizing a combination of mesh refinement, turbulence modeling, and near-wall treatment strategies. Some turbulent flow simulation models such as low-Reynolds number models or hybrid approaches are usually used to calculate the flow distribution in the complex buffer layer area. These turbulence models usually use damping functions or blending techniques to calculate velocity changes from the viscous sub-layer to the log-law layer.

**Log-law layer (30< y+ < 500):** In this layer, both viscous and turbulent effects are important. The velocity distribution is:

Von Karman’s constant (*κ*) is approximately 0.4 and *B* is an empirical constant, typically around 5.5.

## y+ graph

In the next graph, the equations presented in this article are compared with experimental results (points). It can be seen that the equations express the relationship between u+ and y+ well. In the graph, (1/κ)ln(E)=B is used for the equation of the logarithmic region.

Velocity distribution near a solid wall. Adopted from “An Introduction to Computational Fluid Dynamics” by H K Versteeg et al.

## Why Should y+ be Calculated in CFD Simulations?

Depending on which turbulence model you use and what your simulation goal is, your mesh resolution in the neighborhood of the wall needs to have different sizes. One of the key parameters to determine the mesh resolution is y+. You can easily calculate y+ using the y+ calculator in cfdstreamline.

Before simulation, calculate the y+ value for CFD simulation using problem parameters. Then, use two methods to determine the resolution of the mesh next to the wall:

**Wall functions approach:**Compared to other methods, this method has a coarser mesh, which reduces its computational expense. In this method, the wall functions that have been described so far in this article and based on experimental results are used. For complex flows with flow separation or high pressure gradients, this method is less accurate.**It is recommended to use this method, the center of the first mesh cell should be at 30 < y+ < 300****Near-wall model approach (low-Reynolds number modeling**): In this method, the viscous sublayer is simulated with a fine mesh in the area next to the wall where the viscous force is dominant. This method provides proper accuracy in simulating complex flows and flow separation. To achieve high accuracy results, this method**requires y+ values of approximately 1 or less**. Although this method has high accuracy, it requires high computing power due to the small mesh. This method is recommended when your goal is to measure forces on walls

This mesh resolution is suitable based on low-Reynolds number modeling. The velocity in the range of the red curve is calculated with this method. Adopter from simscale.

This mesh resolution is suitable based on the wall functions approach. The velocity in the range of the red curve is calculated with this method. Adopter from simscale.

The Standard k-ε model is recommended for simulating free stream flows, but it is incapable of simulating the flow around the walls, so in this turbulence model, wall functions are usually used for calculations near the walls. On the other hand, the k-ω SST (Shear Stress Transport) model is known for its ability to simulate flows around walls.

To achieve maximum accuracy with k-ω SST, a y+ value for k-omega SST less than 1 is recommended although larger y+ values can be used at the cost of reducing the accuracy of the results. After completing the simulation, you can check the size of the y+. If the resulting y+ shows that the mesh resolution was not suitable, you can redo the simulation.

## Example

A fluid (Air at 20°C) flows over a flat surface. Calculate the dimensionless wall distance (y+) using the following parameters:

Free-stream velocity (*U∞*) is 10 m/s, plate length (*L*) is 1 m, distance of first grid point from the wall (*y*) is 0.0001 m, air density (*ρ*) is 1.204 kg/m³, dynamic viscosity of air (*μ*) is 1.825 × 10⁻⁵ kg/(m·s), and kinematic viscosity of air is (*ν *= *μ/ρ*) is 1.516 × 10⁻⁵ m²/s.

The Reynolds number is:

The skin friction coefficient using the Blasius formula is:

The wall shear stress is:

The friction velocity is:

Finally, y+ is:

In ANSYS Fluent, in the surface integrals section, after simulation, you can extract the size of y+ on all boundaries and walls.

## y+ Values for Different Turbulence Models in ANSYS Fluent

ANSYS Fluent is designed by competent specialists and is constantly being updated. Simulation of the near-wall region, boundary layer, and wall functions have always been among the biggest challenges in CFD and turbulent flow simulation. ANSYS Fluent has consistently demonstrated its capability in these areas. In all turbulent flow simulation models, Fluent’s algorithm is often more advanced than users might expect, and even if the user doesn’t design many mesh resolution points correctly, Fluent can still produce reasonable results. However, it is recommended to follow the guidelines about y+ discussed in this article and adjust mesh resolution accordingly for optimal accuracy.

In the following figure, you can see that ANSYS Fluent is capable of simulating a wide range of viscous models, and for each of these, it offers detailed options for near-wall treatment. The selection of an appropriate model and its correct settings are typically based on previously validated simulation work or the user’s experience in simulating turbulent flows.

In the viscous model settings of ANSYS Fluent, the near-wall treatment section provides users with numerous options to adjust the viscous equations near the wall.

Our experts at CFDLAND have completed numerous academic and industrial projects utilizing ANSYS Fluent for CFD simulations. They have a lot of experience in simulating near-wall fluid behavior and can validate results against previous simulations or experimental data. For assistance with your CFD projects, please visit our ORDER ANSYS Fluent Project page.

## Conclusion

To study fluid flow near solid walls, the dimensionless quantity y+ was defined and wall function was introduced using it. This function was compared with the experimental results in this article and we saw that its results are reliable and accurate. This function is used in many turbulent flow simulations, many of these turbulent flow simulations methods and their suitable mesh size are defined using y+. In some cases, wall function is not suitable for simulation and other methods are used which we have discussed.

**more information: **

Dimensionless Numbers in Fluid Mechanics