2D LES simulation of turbulent jet
 

Hello all,

Im a beginner in Fluent and CFD so please bear with me.

Im trying to run a LES simulation for turbulent jet.

My domain is attached. Its a 0.1 m x 0.15 m rectangle. My inlet is 0.01 m at the bottom of the domain as seen in the picture. I constructed a uniform mesh using ICEM. My grid is 216 x 328. I found my smallest cell size to be 0.00043 (not really sure if this is correct or not).

In Fluent:
Pressure-based solver was selected
Transient was selected
Energy was turned on
Large-Eddy Simulation (LES) was selected and the Kinetic Energy Transport model was selected

Boundary Conditions:
'AH and GF' as WALLS, default options

'HG' as Velocity inlet = Velocity in the Y-direction = 1 m/s, Spectral Synthesizer is chosen. Turbulent Intensity set to 7.07 % and Hydraulic Diameter set to 0.01. I calculated the intensity using this equation I = 0.16*Re^(-1/8) --Provided by fluent manual. Subgrid Kinetic Energy left as 1 m2/s2. Temperature changed to 293 K

'AB, FE, BCDE' as Pressure outlet, default options

SIMPLE scheme was selected.
Gradient: Least square cell based
Pressure: Body force Weighted
Momentum: bounded Central Differencing
Subgrid Kinetic Energy: Second order upwind
Transient Formulation: Second order implicit

Under-Relaxation factors were left default.
All Residuals were changed to 10^-6

Using Standard Initialization, the solution was initialized from the inlet


Now this is where my questions starts:
a) I choose Kinetic Energy Transport model so Subgrid Kinetic Energy will be calculated, is this correct?
b) Is the method that I used to calculate the Turbulent Intensity correct?
c) Do I have to calculate the Subgrid Kinetic Energy in the inlet? If yes, how do I calculate it?
d) Was choosing SIMPLE a good choice?
e) Any comments on the spatial discretization methods used?
f) Should I change the Under-Relaxation factors?
g) Is it correct to initialize the solution from the inlet?

Moving on to the time step size, I read that the time step size< deltax/u
where deltax is the smallest cell size and u is the velocity. Therefore, mine should be 0.00042 ------ Is this correct?

How do I choose the Max iteration/Time step?? I read in this thread (http://www.cfd-online.com/Forums/flu...past-cube.html) that I have to run a RANS simulation first. Im not sure what to do here to be honest.

f) What does the Courant Number have to to do with the time step size? I couldn't find it really.


Sorry for the long thread/questions.

Any help will be greatly appreciated

Thank you.
Adnan

Hi,

my very first question is: why do you want to run a 2D LES? With LES you are solving a portion of the turbulent spectrum, and because turbulence is an inherently 3D phenomenon, I am not sure that a 2D LES makes any sense.

For the discretization schemes: SIMPLEC with rather high URFs works fine from my experience. It is recommended to use BC or BCD schemes for flow equations (upwind schemes are too diffusive) and upwind schemes (SUO, QUICK, MUSCL) for scalars.
Also, you should use a node-based scheme for gradient.

I strongly suggest you to compute an initial RANS solution (e.g. with std k-eps) and then start your LES using RANS results as initial condition.

The Courant number is defined as: C = u*deltaX/deltaT and should be less then Cmax (Cmax can be one but usually it depends on the nature of the problem and on your settings).

Determine the correct mesh size for LES simulation is tricky. There is no such thing as mesh independence in LES. The more your refine your grid, the more you should tend towards DNS (if your simulation is set up correctly). As a rule of thumb 80% of the turbulent kinetic energy has to be solved. A very rough estimation of the grid size is to consider the integral length scale l=k^(3/2)/eps and make sure that you have a reasonable number of grid points within it.

Hope this can help

Andrea

Hi,

I reason Im carrying out a 2D LES is because I want to make sure that I can get reasonable/correct results.

Can you walk me through how to calculate integral length scale? How do I obtain k and eps?

Im sorry but I dont have anyone to help me :(

you can evaluate l=k^3/2/eps from a RANS simulation and the check the ratio delta/l (where delta is your grid size). You can use the attached picture (from an ANSYS presentation) as a rough guideline http://picpaste.com/LES-AW3ALHq3.png

What about the rest of my input? Is it correct?

I think the boundaries are too closed to the input; pressure outlet could be true at the very first time steps, but as soon as the jet develops into the domain I think that these boundaries are not correct.

Do I have increase my domain to 0.1 x 0.3 for example?

How do I know the best distance? is there an equation for it?