[gemxx]

Hi everyone,

My question is about wall y+ function and courant number stabilization criteria.

I analyze turbulent flow past over a submerged body.
Because of high velocity and sharp edges, I have to use very small sized grid for the first cell near the body surface to obtain below 1 of y+ value.
The first cell size is about 1.5x10^-6 m.

When I use this size for the first cell, it is necessary to use too small time step size to obtain about 1 of Courant Number.
Flow velocity is 7.15 m/sn. For this situation, the time step size should be about 2.0x10^-7 to obtain Courant number(CL) =1.
But I have limited computer sources. Therefore, it seems impossible for me.

As I understand, I have two options now.

1-I'll select a bigger first cell size. In such a case, the wall y+ value will be bigger than 1. But I can obtain CL value of 1 by using a bigger time step. This means shorter analyze time for me.

2-I'll select a bigger time step. In such a case, the courant number will be bigger than 1. But I can obtain wall y+ value of 1. This means shorter analyze time for me, as well.

I tried two options. The convergence is better for the first option.
I use implicit unsteady and detached eddy simulation for analyses.

Do you think which one I should choose?

[FMDenaro]

Originally Posted by gemxx

Hi everyone,

My question is about wall y+ function and courant number stabilization criteria.

I analyze turbulent flow past over a submerged body.
Because of high velocity and sharp edges, I have to use very small sized grid for the first cell near the body surface to obtain below 1 of y+ value.
The first cell size is about 1.5x10^-6 m.

When I use this size for the first cell, it is necessary to use too small time step size to obtain about 1 of Courant Number.
Flow velocity is 7.15 m/sn. For this situation, the time step size should be about 2.0x10^-7 to obtain Courant number(CL) =1.
But I have limited computer sources. Therefore, it seems impossible for me.

As I understand, I have two options now.

1-I'll select a bigger first cell size. In such a case, the wall y+ value will be bigger than 1. But I can obtain CL value of 1 by using a bigger time step. This means shorter analyze time for me.

2-I'll select a bigger time step. In such a case, the courant number will be bigger than 1. But I can obtain wall y+ value of 1. This means shorter analyze time for me, as well.

I tried two options. The convergence is better for the first option.
I use implicit unsteady and detached eddy simulation for analyses.

Do you think which one I should choose?

You are considering two different things. The number of cells within y+1 says how good is the resolution of the boundary layer, while the cfl is a ratio between the numerical time step and the physical time in which a particle cross the cell with the proper convective cell velocity.

Often in simulation of turbulence we accomplish both constraints

[gemxx]

Thank you @FMDenaro for your reply.

I know it is better for me to accomplish both constraints.
But I have to choose one of them because of my computer's computational capacity.

Which one is the most important for the accuracy of results?

[FMDenaro]

Originally Posted by gemxx

Thank you @FMDenaro for your reply.

I know it is better for me to accomplish both constraints.
But I have to choose one of them because of my computer's computational capacity.

Which one is the most important for the accuracy of results?

You cannot in general make a choice, the numerical stability constraint is in general a function of the cfl and the cell Re number, this latter being strictly related to the value of y+ close to the wall. Therefore, you can relax the time step only if you enlarge the grid size. When you do that you will see that the BL is no longer resolved and you need to use a different approach in setting the BCs, that is using wall-modelled BCs. But doing this way you can no longer think to compute some quantities as the viscous drag.
This is a general framework valid especially for DNS/LES/URANS, however you can approach directly a RANS formulation, in this case the time step has no physical meaning as you solve for the steady state and you can just focus on the y+ values to resolve the BL.

[LuckyTran]

Originally Posted by gemxx

Thank you @FMDenaro for your reply.

I know it is better for me to accomplish both constraints.
But I have to choose one of them because of my computer's computational capacity.

Which one is the most important for the accuracy of results?

You should still do the mesh sensitivity study and time-step size sensitivity study anyway and when you do, you will learn the answer to your question.

There is no general rule for all scenarios, you need to choose. If you don't care about resolving boundary layers, you can even run a y+ ~100. The question is, do you care about resolving the boundary layers? No one here knows what criteria you are using to determine accuracy to help you. You mention accuracy of results, but what are the results you are aiming to achieve? Still, we can't predict what will happen. Do the sensitivity study if you need to know!

[gemxx]

Originally Posted by LuckyTran

You should still do the mesh sensitivity study and time-step size sensitivity study anyway and when you do, you will learn the answer to your question.

There is no general rule for all scenarios, you need to choose. If you don't care about resolving boundary layers, you can even run a y+ ~100. The question is, do you care about resolving the boundary layers? No one here knows what criteria you are using to determine accuracy to help you. You mention accuracy of results, but what are the results you are aiming to achieve? Still, we can't predict what will happen. Do the sensitivity study if you need to know!

Actually, I did the mesh sensitivity study. Despite I used more relaxed grid cells, I obtained reasonable results with the experimental data in literature.
The wall y+ is about 30. I avoid to select wall y+ between 5 and 30 (buffer layer).
Could you tell me the important points related to wall y+? I use "all wall y+" module of Star ccm+ and it is written in tutorial that wall y+ from 5 to 30 can be used for all wall y+ module and blended approach creates a reasonable solutions for 5<y+<30. What is the meaning of this?
Courant number is important for me and I have to select smaller time step size as soon as possible to capture vortex structures. Thats why, I decided to relax the grid size. Do you think that I am on the right road?
Thank you very much.

[FMDenaro]

As I wrote above, such high value for the first node close to the wall requires to prescribe wall-modelled BCs., you cannot prescribe the no-slip condition. If you are doing that, the results behind the body can be reasonable. Of course, you cannot predict the drag due to the stress

[LuckyTran]

Originally Posted by gemxx

I use "all wall y+" module of Star ccm+ and it is written in tutorial that wall y+ from 5 to 30 can be used for all wall y+ module and blended approach creates a reasonable solutions for 5<y+<30. What is the meaning of this?

There is a high y+ wall function valid only for high y+ and low y+ wall function valid only for low y+. For general purpose CFD these wall functions are crap since it requires the user to supply grids that globally satisfy wall y+ > 30 or globally satisfy wall y+ < 5. People don't like to do CFD this way. The all wally+ wall function uses a cute elliptic blending function to smooth these wall functions into one wall function so that you can use it on any mesh.

Originally Posted by gemxx

Courant number is important for me and I have to select smaller time step size as soon as possible to capture vortex structures. Thats why, I decided to relax the grid size. Do you think that I am on the right road?
Thank you very much.

The Courant number less than some arbitrary number criteria is for stability, not necessarily accuracy. Going to a coaser grid gives you a smaller Courant number, but you lose spatial resolution. It is unclear without testing whether the improved numerical stability due to having a smaller Courant number gives you any better or worse results. Of course you won't find any vortex that close to a wall if that is the only region where the grid is being coarsened. You are also using implicit time-stepping, which is much more robust against these numerical oscillations (due to the application of under-relaxation). What is more important is the time-step size. So probably you made a reasonable choice by accident.

[akucuk]

I might not be the right person to answer your question because im a newbie in CFD. So i hope expert people will correct me if i'm wrong.

Why do you calculate the courant number from the first cell? Doesnt the first cell supposed to have less velocity due to its y+ value. Im not really sure about what im saying but if i were you i would calculate courant number for the freestream part of the mesh.

Aykut

[FMDenaro]

Originally Posted by akucuk

I might not be the right person to answer your question because im a newbie in CFD. So i hope expert people will correct me if i'm wrong.

Why do you calculate the courant number from the first cell? Doesnt the first cell supposed to have less velocity due to its y+ value. Im not really sure about what im saying but if i were you i would calculate courant number for the freestream part of the mesh.

Aykut

Indeed the cfl number is local and is required to control it everywhere. But in a viscous problem, depending on the type of expòicit discretization a complex relation cfl(Re_h) could be involved and, generally, such constraint region requires the cfl to be quite smaller than 1 when the value Reh is small.

[LuckyTran]

Originally Posted by akucuk

Why do you calculate the courant number from the first cell? Doesnt the first cell supposed to have less velocity due to its y+ value. Im not really sure about what im saying but if i were you i would calculate courant number for the freestream part of the mesh.

Aykut

You have the right idea. But given the amount of time that has passed and that results have already been obtained, I just assumed that the actual Courant number field was available and there's no longer any need to guess what it is. So I assumed that mesh coarsening was done where the Courant number was small.

[akucuk]

Originally Posted by FMDenaro

Indeed the cfl number is local and is required to control it everywhere. But in a viscous problem, depending on the type of expòicit discretization a complex relation cfl(Re_h) could be involved and, generally, such constraint region requires the cfl to be quite smaller than 1 when the value Reh is small.

I get the concept but he says that the velocity is 7.15 m/s which i think is not a possible velocity value for a first cell near wall. That forced me to think that he calculated the courant number for the fully developed turbulent region.

I also doubt that if you calculate courant number for the outer region(referring to y+ graph) it should be larger than inner layer of mesh because the velocities are always less in inner layer than the outer layer. Or at least it could be a nice approach to guess the whole cfl condition in my humble opinion.

[FMDenaro]

Originally Posted by akucuk

I get the concept but he says that the velocity is 7.15 m/s which i think is not a possible velocity value for a first cell near wall. That forced me to think that he calculated the courant number for the fully developed turbulent region.

I also doubt that if you calculate courant number for the outer region(referring to y+ graph) it should be larger than inner layer of mesh because the velocities are always less in inner layer than the outer layer. Or at least it could be a nice approach to guess the whole cfl condition in my humble opinion.

The velocity should be scaled by U* to get u+ (in the viscous sublayer proportionla to y+). However, the cfl number is actually a multidimensional parameter, it is not correct to control separately the cfl in each direction separately. And, finally, the viscous stability parameter can be dominant, especially if the turbulence model is of eddy viscosity type.

[LuckyTran]

Originally Posted by akucuk

I get the concept but he says that the velocity is 7.15 m/s which i think is not a possible velocity value for a first cell near wall. That forced me to think that he calculated the courant number for the fully developed turbulent region.

It's very common that people use the bigger velocity and smaller cell size to calculate a bigger Courant number, i.e. to get a conservative estimate.

Anyway, at this point they should be using the actual courant number calculated from local cell size and local velocity and we shouldn't be wondering how they estimated it the first time.