In recent posts in our series of Turbulence Modelling posts, we have covered boundary layer theory and touched on some useful meshing and post-processing guidelines to check you are appropriately resolving the boundary layer profile. Today we will consider three critical questions that are often asked by CFD engineers when developing or refining a CFD simulation:

*- Am I using the correct turbulence model for the type of results I am looking for?*

*- Do I have an appropriate Y+ value and a sufficient number of inflation layers?*

*- Am I using the right wall function for my problem?*

This topic is so important because we know that in turbulent flows the velocity fluctuations within the turbulent boundary layer can be a significant percentage of the mean flow velocity, so it is critical that we capture these effects with accuracy. A Reynolds averaging approach using turbulence models will provides us with an estimate of the increased levels of stress within the boundary layer, termed the Reynolds stresses. In order to appreciate the use of wall functions and the influence of walls on the turbulent flowfield, we should first gain familiarity with the composite regions of the turbulent boundary layer:

In the laminar sub-layer region (Y+ < 5) inertial forces are less domineering and the flow exhibits laminar characteristics, which is why this is known as the low-Re region. Low-Re turbulent models (e.g. the SST model) aim to resolve this area and therefore require an appropriate mesh resolution to do this with accuracy. This is most critical for flows with a changing pressure gradient where we expect to see separation, as observed below.

In the law of the wall region, inertial forces strongly dominate over viscous forces and we have a high presence of turbulent stresses (this is known as the high-Re composite region). If using a low-Re model, the whole turbulent boundary layer will be resolved including the log-law region. However, it possible to use semi-empirical expressions known as **wall functions** to bridge the viscosity-affected region between the wall and the fully-turbulent region.

The main benefit of this wall function approach lies in the significant reduction in mesh resolution and thus reduction in simulation time. However, the shortcoming lies in numerical results deteriorating under subsequent refinement of the grid in wall normal direction (thus reducing the Y+ value into the buffer layer zone). Continued reduction of Y+ to below 15 can gradually result in unbounded errors in wall shear stress and wall heat transfer (due to the damping functions inherent within the wall function approach).

Bearing all of the above in mind, and keeping our eye on finding the right balance between accuracy, stability and speed, we can tackle a wide variety of CFD problems using the following guidelines:

**What results am I interested in** **and am I using the right turbulence model?**

If our aim is to accurately predict the boundary layer velocity or thermal profile, or if the developing boundary layer will tend to separate (due to a changing pressure gradient – and not because of sharp edges or discontinuities in the geometry), then we recommend the use of a low-Re model. Low-Re models are also required for accurate pressure-drop or drag calculations. We highly recommend the use of the Shear Stress Transport (SST) model, but all *ω*-based models or *ε*-based models with enhanced wall treatment may be used. For high speed external aerodynamic flows, the one-equation Spalart-Allmaras model (with Y+ < 2) may also be considered to reduce the computational time. Alternatively, for flows where wall-bounded effects are not a priority, or if separation is expected to occur only due to sharp changes in the geometry, an *ε*-based wall function approach is more than sufficient. In ANSYS CFD, all *ω*-based models and the SST model are capable of resorting to a wall function formulation (automatic wall treatment) in the presence of coarse mesh resolutions near the wall without any further user input. Wall function models are also useful for calibrating our CFD models, due to the decreased simulation time.

**What is my Y+ value and do I have a sufficient number of prism layers?**

When using low-Re models or any models with enhanced wall treatment, the average Y+ value should be on the order of ~1 to ensure we are capturing the laminar sub-layer. When using wall function models, the Y+ value should ideally be above 15 to avoid erroneous modelling in the buffer layer and the laminar sub-layer. High quality numerical results for the boundary layer will only be obtained if the overall resolution of the boundary layer is sufficient. This requirement in some cases is more important than achieving certain Y+ values. The minimum number of cells to cover a boundary layer accurately is around 10, but values of 20 are desirable. The total thickness of the prisms should be implemented such that around 15 or more nodes are actually covering the boundary layer. Our next post in this series on the turbulent boundary layer will cover a very useful and practical technique to post-process the resolution of the boundary layer, and offer insight into modifications required to improve accuracy.

**Am I using the right wall function?**

In ANSYS CFD, all turbulence models are y-plus independent. However selecting the *most appropriate* wall function is dependent on level of refinement of our wall adjacent mesh, or the relative scales in our flow. Use of the standard wall function (*ε*-based models) implies that our boundary layer mesh lies entirely within the log-law region of the boundary layer. For industrial applications, this in fact might be difficult to achieve due to varying geometrical and velocity scales associated with our model – and therefore grids inherently designed with arbitrary refinement. We highly recommend the use of the scalable wall function, which offers an elegant solution to this ambiguity often encountered. This wall function virtually displaces the mesh to a Y+ ~ 11.225 (transition to the log-law composite layer) irrespective of the level of refinement, thereby avoiding the erroneous modelling of the laminar sub-layer and buffer region. It is also important to note that for grids designed with a Y+ > 11.225, the scalable wall function will provide identical results to the standard wall function. Enhanced wall treatment may further be selected for *ε*-based models on refined low-Re grids, and is also formulated such that it can perform well for meshes of intermediate resolution. However the use of enhanced (or non-equilibrium) wall treatment for low-Re modelling of the turbulent boundary layer is generally not recommended and more confidence in our solution can be obtained by selecting a suitable *ω*-based formulation, such as the SST model.

April 16, 2013

I have read your article and there is one think that I do not understand.

"Scalable wall function - This wall function virtually displaces the mesh to a Y+ ~ 11.225 (transition to the log-law composite layer) irrespective of the level of refinement, thereby avoiding the erroneous modelling of the laminar sub-layer and buffer region."

Does this mean that using Scalable wall function the mesh will be rebuilt in the way to consist both phenomena: laminar and transition flow?

April 22, 2013

If your model has varying geometrical or velocity scales, then consequently your grid and near-wall refinement will have varying levels of resolution. To maintain consistency in our modelling approach the scalable wall function will virtually displace the near-wall mesh to a y+ value of 11.225, which is the transition to the log-law region. This is necessary since epsilon-based models are not ideal for modelling the laminar sub-layer and the scalable approach internally adjusts the mesh to ensure this region is not resolved. The scalable approach is the default option in ANSYS CFX and is an available option in ANSYS Fluent. The scalable wall function will not capture laminar or transitioning flow, as it is purely a turbulent wall function approach. To model aerodynamic flows with laminar-to-turbulent transition, we encourage the use of the SST transition model. This low-Re model requires fine resolution in the near-wall region due to the complexity of transitioning flow.

July 18, 2013

Hi experts,

You stated that with Scalable Wall Function method, it virtually displaces the mesh to a Y+ ~ 11.225. And on top up the page there is figure showing buffer layer yplus between 5 to 30.

So it seems somehow wrong to place first layer in buffer layer!

Can you explain more?

Thank you in advance.

July 30, 2013

The scalable wall function will displace the mesh to a Y+ ~ 11.225 since this is noted as the numerical transition point from when a boundary layer operates in the laminar sub-layer to the turbulent log-law. It is simply a virtual scale of first cell height so that the solver internally operates as if we are in the log-law region and not within the laminar sub-layer.

September 26, 2013

how does ansys calculte in the near wall region ?is it like this :at the first cell,use emprical correlation,and from the second cell solving k-e equation ?If it is like this ,why we need sufficient boundary layer?

thank you for your reply..

October 13, 2013

hiiii...

My geometry is wing of airfoil cross section inside a rectangular box domain. I am using Standard k-e model. what should be my y+? Does k-e model is good or i should move to another model.

December 9, 2013

Hi,

I am modeling a shell and tube heat exchanger and i am having problem with pressure drop on shell side. My analytical calculations give pressure drop of 470 Pa while fluent gives 2300 Pa. Average Y+ value on tube walls is 20. Turbulence model is K-e with standard wall functions. Kindly help me in this issue.

Thanks.

January 3, 2014

It is difficult for us to comment on this, since we do not have an understanding of the geometry or your choice of boundary conditions. Nor can we assume that your analytic calculations are in fact valid for the problem setup. The discrepancy in the result is likely not to be solely due to mesh resolution, rather it is likely to do primarily with the choice of boundary conditions. Our advice would be to attempt one of the tutorials from the help guide which address heat transfer to gain an understanding of a representative problem setup.

December 23, 2013

Dear Leap Group:

I saw we explained "Low-Re models are also required for accurate pressure-drop or drag calculations. We highly recommend the use of the Shear Stress Transport (SST) model, but all ω-based models or ε-based models with enhanced wall treatment may be used." in part "What results am I interested in and am I using the right turbulence model?",

But we said "However the use of enhanced (or non-equilibrium) wall treatment for low-Re modelling of the turbulent boundary layer is generally not recommended and more confidence in our solution can be obtained by selecting a suitable ω-based formulation, such as the SST model."

I wonder if these two speaking are contradictory for Enhanced Wall Treatment used in Low-Re? So how we to understand Enhanced Wall Treatment for solving boundary layer?

January 3, 2014

It is necessary to understand the limitations and range of applicability of the eddy-viscosity turbulence models. No single model can be applied to all problems of interest - however the omega-based models and in particular the SST model are often preferred, particularly because of their favourable wall treatment. They are relatively more robust near the wall, and the y-plus insensitive treatment is facilitated through the automatic wall treatment. They are also relatively easier to combine with additional physics, such as transition. There is still ongoing development for epsilon-based models, in particular the y-plus insensitive treatment through the enhanced wall treatment and for many problems the use of realizable k-epsilon with enhanced wall treatment, for instance, will provide a valid result. In this post we aimed to provide our recommendation for a baseline model to capture boundary layer flows for a wide range of applications, and due to its robustness, we have opted for the SST model.

February 26, 2014

hi,

we use a wall function for boundary layer so why do we need to have some nodes in this region?

my English is not good enough.

thanks

March 7, 2014

We respectfully suggest that you re-read this post and other related posts on wall functions/full resolving the boundary layer on our Blog.

July 28, 2014

Hello,

In transient simulation of a flow, the Y+ is not a constant value and alters during time. Which Y+ should I consider to evaluate the cell size near the wall?

Thanks for your help.

October 9, 2014

Hi Mohsen,

The y+ value is not constant because now your friction velocity distribution on your wall is changing over time. Rather than taking the y+ distribution at a specific timestep, you should be taking the transient average of the y+ over the simulation time

Regards,

LEAP CFD Support

August 5, 2014

Hi experts,

If I want to use non-equilibrium wall function, what's the range that is suitable to the non-equilibrium wall function ? whether is it suitable as long as the value of Y+ is larger than 11.25 ? I want to simulate the process of wedge of water-entry,could you please give me some advice on choosing the wall function ? what I most concern is the splashing during the the process of wedge of water-entry.

Thank you so much.Best wishes for you and I am longing for you reply.

October 9, 2014

Hi,

The non-equilibrium wall function is useful for log-law resolution, and is different from the standard wall function is that it can partly take into account the effects of pressure gradient. However its scope of applicability begins to fall apart when you take into account severe pressure gradients leading to boundary layer separations, and strong body forces which your case will be subject to. In this case, it is preferred to use the enhanced wall treatment approach with y-plus values ~1.

Regards,

LEAP CFD Support

November 3, 2014

Dear LEAP experts,

Thanks a lot for your posts!

As I'm normally involved with internal flows simulation, by your suggestion I chose to switch from ke to kw-SST, as sometimes I can see some flow detaching and I'm interested in heat transfer too.

But I still have some confusion about some terms normally used when speaking about turbulence (maybe synonymous), and for the physics.

Referring to “Estimating first cell Height for y+”:

When I have to solve the viscous sub-layer in order to have an y+ of 1, why should I still use an approximation like a wall function? I mean, if I have a y+ of 1, it means that surely I'm really close to the wall with my calculation point, so why should I use a wall function to model the behaviour of the flow? If I would be able to add more layers near the wall, are NS equations well discretised as well at the wall anyway, and so I could switch off wall functions?

Thanks a lot

Mike

January 22, 2016

Wall functions are used when the inflation layers do not sufficiently resolve the boundary layer. If you resolve the viscous sublayer, wall functions can still be used for the turbulent layer, depending on the y+ value. One of the benefits of the k-w SST model is that it will automatically use the low-Re formulation in the viscous sublayer and will use the wall function if the cell height is in the log-law layer.

April 16, 2015

Hello experts

I am designing a CD nozzle for a turbine. I meshed it in ICEM CFD.I took k-epsilon model with standard wall functions. I need to find the pressure and temperature at the walls of CD nozzle. Which wall function should I choose to get correct pressure value at the walls and get the correct velocity value at the exit?

January 22, 2016

To obtain accurate pressures and velocities, the recommended turbulence model would be the k-w SST. You will also need to fully resolve the boundary layer, keeping in mind that if Pr>1 for your problem, the thermal sublayer will be much thinner than the momentum sublayer. You boundary layer mesh will need to be adjusted accordingly so that both the thermal and momentum sublayers are captured appropriately.

April 28, 2015

Hi

I've tried to simulate a classical problem of flow and heat transfer in a circular tube with constant heat flux, radius of 10mm and 60mm length. I've used the periodic boundary condition, K-epsilon model with standard wall function and the Reynolds number is between 10000 to 40000. When I use the finer mesh, the friction factor and Nusselt increase drastically and diverge from the analytical results. This problem is more serious for low Reynolds (10000

January 22, 2016

The k-w SST model is likely a better choice for your problem as k-w models are known to outperform k-e models with respect to boundary layer flows. The fact that mesh refinement causes even further deviation from the analytical results supports this as the closer to the wall you refine, the more pronounced the deficiencies in the k-e model become. The SST model, combined with the other recommendations from this blog series should improve your simulation.

June 21, 2015

I have two question related to Y plus.

1- I am trying to have y+<5 while using K-epsilon method (enhanced wall) in a 5 m pipe. My y+ results give a value of less than 5 but the earlier values are about 8 and then it downs to less than 3 severely. Is this ok or not? Y plus value must be less than 5 throughout the geometry wall?

2- My goal is to find pressure drop throughout a pipe. The amount of pressure drop changes with quality of mesh even for the Y plus value less than 5. For example for the y+=3 I have dp=3600 Pa and for y+=0.5 I have dp=3400 Pa. which one is true?

Thank you for your attention to my request

September 24, 2015

Hi Ali,

1) For enhanced wall functions, the average y+ value needs to be around 1 in order to ensure the laminar sublayer is captured.

2) It is important to verify any model through a mesh independence study. Please see http://www.computationalfluiddynamics.com.au/convergence-and-mesh-independent-study/ for further details