[medaouarwalid]

Hi, i want to generate a good grid for large eddy simulation using the taylor micro scale. I found a relation wich includes reynolds numer and kinematic viscosity and velocity fluctuation. But i dont know how to get velocity fluctuations

[FMDenaro]

Originally Posted by medaouarwalid

Hi, i want to generate a good grid for large eddy simulation using the taylor micro scale. I found a relation wich includes reynolds numer and kinematic viscosity and velocity fluctuation. But i dont know how to get velocity fluctuations

A grid resolving up to the Taylor micro-scale is practically a DNS grid...
The grid filter in LES has to lie in the inertial range, at a lenght scale that is at least one order of magnitude greater than the Taylor lenght.

[medaouarwalid]

Originally Posted by FMDenaro

A grid resolving up to the Taylor micro-scale is practically a DNS grid...
The grid filter in LES has to lie in the inertial range, at a lenght scale that is at least one order of magnitude greater than the Taylor lenght.

I thaught that a grid up to kolmogorov scale is the one wich is pratically a DNS grid

[FMDenaro]

Originally Posted by medaouarwalid

I thaught that a grid up to kolmogorov scale is the one wich is pratically a DNS grid

The Taylor microscale is the largest of the dissipative lenght scale, at that level of resolution you are practically starting using a DNS grid. The Kolmogorov is the smallest scales but in a practical simulation you will see no relevant differences between the two grids.

[medaouarwalid]

Originally Posted by FMDenaro

The Taylor microscale is the largest of the dissipative lenght scale, at that level of resolution you are practically starting using a DNS grid. The Kolmogorov is the smallest scales but in a practical simulation you will see no relevant differences between the two grids.

Is there an other known scale used by the LES larger than taylor microscale but not too large to loose the advantage of the LES ?

[FMDenaro]

Originally Posted by medaouarwalid

Is there an other known scale used by the LES larger than taylor microscale but not too large to loose the advantage of the LES ?

You are free to set the grid filter at an interval of scales in the inertial range. That is valid for homogenous directions, in case of wall confined flows the grid is as fine as a DNS in case you resolve the BL.

[medaouarwalid]

Originally Posted by FMDenaro

You are free to set the grid filter at an interval of scales in the inertial range. That is valid for homogenous directions, in case of wall confined flows the grid is as fine as a DNS in case you resolve the BL.

From what I understand with LES method, mesh size has to be in the inertial zone so it's smaller than large scale phenomena and bigger than smaller scales that would be filtered be the model. In this region energy is still transferred from larger to smaller scales.
Now ,which is the parameter to caracterise the grid, the smalest size of the edge or the face or the celle , and how i can know if my grid is still in the inertial zone ?

[FMDenaro]

Of course you first need to consider the flow problem you want to simulate...
you can read this paper https://www.google.it/url?sa=t&rct=j...9Xi_qA&cad=rja

[medaouarwalid]

Originally Posted by FMDenaro

Of course you first need to consider the flow problem you want to simulate...
you can read this paper https://www.google.it/url?sa=t&rct=j...9Xi_qA&cad=rja

I read it befor, but i still have difficulties to determine the inertial zone of my flow problem ( it is a ventilation problem: seven air jets in a room) could you give explain to me ?

[FMDenaro]

Originally Posted by medaouarwalid

I read it befor, but i still have difficulties to determine the inertial zone of my flow problem ( it is a ventilation problem: seven air jets in a room) could you give explain to me ?

As your post starts with the Taylor microscale, you can consider that a grd size greater than that lies at the end of the inertial sub-range. In homogeneous-isotropic flows, the characteristic Reynolds number is computed in terms of this lenght scale. A cell Reynolds number of O(10) is a good choice.
In case of confined flows, you have to consider the distance from the wall (the so called y+) and the Reynolds number is based on the wall velocity. Generally, the grid size in LES resolves the boundary layer (at least 3-4 nodes within y+<1), otherwise wall-modelled bc.s have to be used.

Your flow problem has both walls and jets in air. Chose the Reynolds that characterizes at the best your problem and follow the above criteria. A more detailed estimation of the grid can be done only when all the geometries and inflow parameters are defined. Then, a relevant issue is the goal of the simulation. This tell you the degree of resolution the grid must have in some region.

[medaouarwalid]

Originally Posted by FMDenaro

As your post starts with the Taylor microscale, you can consider that a grd size greater than that lies at the end of the inertial sub-range. In homogeneous-isotropic flows, the characteristic Reynolds number is computed in terms of this lenght scale. A cell Reynolds number of O(10) is a good choice.
In case of confined flows, you have to consider the distance from the wall (the so called y+) and the Reynolds number is based on the wall velocity. Generally, the grid size in LES resolves the boundary layer (at least 3-4 nodes within y+<1), otherwise wall-modelled bc.s have to be used.

Your flow problem has both walls and jets in air. Chose the Reynolds that characterizes at the best your problem and follow the above criteria. A more detailed estimation of the grid can be done only when all the geometries and inflow parameters are defined. Then, a relevant issue is the goal of the simulation. This tell you the degree of resolution the grid must have in some region.

I have only the walls of the nozzles so boundary layers need to be resolved in that area and the rest is wall-modelled b.c right ?
To calculate N the number of nodes In my case i will 2 reylonds numbers to deal with, Relx for wall resolving and Relx for wall modeled likeis mentionned in the topic u sent it to me.
This Relx = (velocity*Lx)/visco , velocity i think is inlet velocity right, so what is Lx in bothe cases ( modeled and resolved b.c) length of the nozzles or length of the room in streamwise direction

[FMDenaro]

Consider the jets, this is the flow problem you want to be well resolved, right? What about your Re numbers? Then the room is just a closed box wherein you do not need to resolve neither dynamic or thermal boundary layers, right?

[medaouarwalid]

Originally Posted by FMDenaro

Consider the jets, this is the flow problem you want to be well resolved, right? What about your Re numbers? Then the room is just a closed box wherein you do not need to resolve neither dynamic or thermal boundary layers, right?

Yes right. I want to calculate velocity and température in the axial direction and also in the radial one, the nozzle has the greatest effect thats why i thought to well resolve in that area. Walls of the room are bot important to me because it is not a confined jet and i even concidered it as pressure outlet.