[medaouarwalid]

Hi, i read that the large eddy simulation (LES) approach is very sensitive to the grid quality and there is no independence otherwise it becam a DNS approache, also it is very sensitive for the numerical methode employed. So how to choose the wright grid, the numerical methode, the initialization methode (hybrid or standard in fluent) and the time step size for calculation ?

[FMDenaro]

Originally Posted by medaouarwalid

Hi, i read that the large eddy simulation (LES) approach is very sensitive to the grid quality and there is no independence otherwise it becam a DNS approache, also it is very sensitive for the numerical methode employed. So how to choose the wright grid, the numerical methode, the initialization methode (hybrid or standard in fluent) and the time step size for calculation ?

I suggest a reading of the book of Sagaut on the LES topics. A much more general presentation can be found in the book of Peric & Ferziger. I also suggest to have the book of Pope for some topics about turbulence.
You can also find some brief notes I wrote https://www.researchgate.net/publica..._Part_I_and_II

[piu58]

> is very sensitive to the grid quality and there is no independence o

There is a huge difference between grid quality and spatial differentiation.

LES may be sensitive to the quality, but that is true for RANS too. It is possible, however, to get a (nearly) grid independent solution with LES.

You should taken into account what LES is developed for: Free shear fluid flow. In the near of walls, assumptions are made, but all in all to a lesser degree as with RANS.

The most problematic cases are the ones where the energy transfer gets doesn't flow from the large to the small eddies, but in the opposite direction. Combustion or chemical reactions are such cases.

[FMDenaro]

Originally Posted by piu58

> is very sensitive to the grid quality and there is no independence o

There is a huge difference between grid quality and spatial differentiation.

LES may be sensitive to the quality, but that is true for RANS too. It is possible, however, to get a (nearly) grid independent solution with LES.

You should taken into account what LES is developed for: Free shear fluid flow. In the near of walls, assumptions are made, but all in all to a lesser degree as with RANS.

The most problematic cases are the ones where the energy transfer gets doesn't flow from the large to the small eddies, but in the opposite direction. Combustion or chemical reactions are such cases.

Yes, in case of confined flows you have two choice: a DNS grid resolution or a RANS-like apporach with wall-modelled BC.s

However, energy backscatter is not a problem using dynamic modelling and scale similarity.

[FMDenaro]

Originally Posted by medaouarwalid

Hi, i read that the large eddy simulation (LES) approach is very sensitive to the grid quality and there is no independence otherwise it becam a DNS approache, also it is very sensitive for the numerical methode employed. So how to choose the wright grid, the numerical methode, the initialization methode (hybrid or standard in fluent) and the time step size for calculation ?

have a look here https://www.google.it/url?sa=t&rct=j...31b35g&cad=rja

[medaouarwalid]

Okay i will read it. A question About the grid , how to judge the grid, about number of elements or about mesh metric like skewness, orthogonal, element quality, aspect ratio ....
For examole two meshes with the same mesh metrics but difference in number of elements, which one is the best ?

[piu58]

> For example two meshes with the same mesh metrics but difference in number of elements, which one is the best ?

All in all you should avoid skew elements , very different element sizes and large changing in element size. This is especial true for regions you are interested in.

A decent simulation includes an examination of dependence of the result from the mesh density. It would be best to simulating with half and double the mesh size. If this is not affordable, at lest a factor of 1,5 should be used.

[medaouarwalid]

Originally Posted by piu58

> For example two meshes with the same mesh metrics but difference in number of elements, which one is the best ?

All in all you should avoid skew elements , very different element sizes and large changing in element size. This is especial true for regions you are interested in.

A decent simulation includes an examination of dependence of the result from the mesh density. It would be best to simulating with half and double the mesh size. If this is not affordable, at lest a factor of 1,5 should be used.

What is the acceptable pourcentage of difference between results, can you give me an average or an interval ?

[piu58]

If you double the node density and get a difference of the main results of let's say 10%, than you have to assume that a even finer mesh would get another 10% and a very very fine mesh again some percents. You are not in a region I would call mesh independent.

Differences of no more than "single percents" (1-3%, maximal 5) should be aspired. If you need to vary some parameters of the geometry or b.c, the chemisty or what else you don't need to perform the mesh analysis for all cases. It is sufficient to investigate a typical one.

[medaouarwalid]

Originally Posted by piu58

If you double the node density and get a difference of the main results of let's say 10%, than you have to assume that a even finer mesh would get another 10% and a very very fine mesh again some percents. You are not in a region I would call mesh independent.

Differences of no more than "single percents" (1-3%, maximal 5) should be aspired. If you need to vary some parameters of the geometry or b.c, the chemisty or what else you don't need to perform the mesh analysis for all cases. It is sufficient to investigate a typical one.

Can i know in advance what grid to begin with, and compare it after with a double and a half ? I ask a lot about the grid because i have a big domaine, it is a room of 4m*4m*2m so i would like to have at least an idea because it takes time to try without any guess

[FMDenaro]

Originally Posted by medaouarwalid

Can i know in advance what grid to begin with, and compare it after with a double and a half ? I ask a lot about the grid because i have a big domaine, it is a room of 4m*4m*2m so i would like to have at least an idea because it takes time to try without any guess

The lenghts of the domain are only one parameter, you have to consider the characteristic velocity that give you the magnitude of the Reynolds number.
Consider then if you need to resolve the boundary layer across the walls.

Just as an example, I solved a problem in a domain of 100m^3 at Re=10^3 using 100^3 grid points. Again, have a look the the paper I linked.

[piu58]

A big domain ist not a big problem if you don't need to resolve small details. That means, if there is only a slow velocity. Regions with high velocity need to mesh finer.

[medaouarwalid]

Originally Posted by FMDenaro

The lenghts of the domain are only one parameter, you have to consider the characteristic velocity that give you the magnitude of the Reynolds number.
Consider then if you need to resolve the boundary layer across the walls.

Just as an example, I solved a problem in a domain of 100m^3 at Re=10^3 using 100^3 grid points. Again, have a look the the paper I linked.

Yes i downloaded it, but i am out now and i am using a phone, i will red it when i go home, i could not hold my self of posting questions i am sorry, the initial reynolds number in my case is 18300 for each jet (i have 7 jets) , velocity is 6.8m/s for each jet also and my big interest is the velocities and temperature in the room , the boundary layers that have a big influence are across the walls of the nozzles that the air go through, but the walls of the room are far from the blowing plane and velocities there are close to zero even pressure is the atmospherique pressure , thats why i concider it like pressure outlet

[FMDenaro]

Originally Posted by medaouarwalid

Yes i downloaded it, but i am out now and i am using a phone, i will red it when i go home, i could not hold my self of posting questions i am sorry, the initial reynolds number in my case is 18300 for each jet (i have 7 jets) , velocity is 6.8m/s for each jet also and my big interest is the velocities and temperature in the room , the boundary layers that have a big influence are across the walls of the nozzles that the air go through, but the walls of the room are far from the blowing plane and velocities there are close to zero even pressure is the atmospherique pressure , thats why i concider it like pressure outlet

Well, you need to refine enough the grid around each jets. I think you need to work initially with some millions of nodes for the whole domain.
But if you need to study only the effect of the jet, you could consider a simplified model, for example a unique jet with a periodic domain.

[medaouarwalid]

Originally Posted by FMDenaro

Well, you need to refine enough the grid around each jets. I think you need to work initially with some millions of nodes for the whole domain.
But if you need to study only the effect of the jet, you could consider a simplified model, for example a unique jet with a periodic domain.

My study is about the multiple jets, and the effect of the interaction between them on the augmentation of rhe mixing between the air jet and the ambiant air of the room

[medaouarwalid]

An other question, if i want lets to compare lets say a configuration of 7 jets to a configuration of 3 jets to find wich configuration gives tje best mixing of air based on température and velocity mesurements, what parameter to fix ( based on diameter of the nozzles and velocity) i can use do the comparaison ? For example to compare a jet wich exit from a nozzle A and an other jet from an other nozzle B, the searchers did the comparaison with keeping the same reynolds number at the nozzles exit. So if the nozzle are not the same, velocity must also not be the same too keep Re equal. But in the case of multiple jets when the number of jet is not the same, how to compare ?

[icornejo]

Originally Posted by medaouarwalid

Can i know in advance what grid to begin with, and compare it after with a double and a half ? I ask a lot about the grid because i have a big domaine, it is a room of 4m*4m*2m so i would like to have at least an idea because it takes time to try without any guess

The element size is strongly dependent of the Re number. To have an estimation of the element size that you need, think that for LES you should go up to the taylor microscale. It means:

l/L = (10/Re)^(-1/2)
Where l is your elements characteristic lenght and L is a characteristic lenght of your domain.

For a 4x4x2m room, with Re ~10^4, you could need easely several tens of millons of elements.





Sent from my SM-T810 using CFD Online Forum mobile app

[icornejo]

Originally Posted by medaouarwalid

Okay i will read it. A question About the grid , how to judge the grid, about number of elements or about mesh metric like skewness, orthogonal, element quality, aspect ratio ....
For examole two meshes with the same mesh metrics but difference in number of elements, which one is the best ?

The two main indicators are the skewness, orthogonal quality and aspect ratio. As you say, if you just make all proportionally finer, your indicators will be the same.

Those indicators are more related with divergence problems that with the grid independence. Grid independence is mostly dependent of the grid size.

Using finer meshes in LES you will obtain more and more details, BUT average quantities should converge to stable values. It means, you can state grid independence calculating U and u' in some relevant points. U is the time-average and u' the standar deviation of the velocity, both at some point(s).

Sent from my SM-T810 using CFD Online Forum mobile app

[FMDenaro]

Originally Posted by icornejo

The element size is strongly dependent of the Re number. To have an estimation of the element size that you need, think that for LES you should go up to the taylor microscale. It means:

l/L = (10/Re)^(-1/2)
Where l is your elements characteristic lenght and L is a characteristic lenght of your domain.

For a 4x4x2m room, with Re ~10^4, you could need easely several tens of millons of elements.




Sent from my SM-T810 using CFD Online Forum mobile app

Well, actually the Taylor microscale is the largest of the dissipative lenght scale, therefore you would resolve almost with a DNS grid resolution...Theoretically, the filter lenght (in other words the grid size) must lie in the inertial range of the spectrum, a region almost without effect of dissipation.