hi,

Can anyone has experience of computing LES chanel flow. I am facing problem during computation. I am not getting signal. If anybody has experience , please share.

thanks...

Hi,

If you carry out a LES compute the turbulent kinetic energy and look carefully how it develops. Initially, it will decrease but after some time it should increase again if the code/model is correct and if you use suitable initial conditions. Are you sure that the Reynolds is correct? Verify that. It is also better to impose initial disturbances with a longer wave length (of the order of a fifth or tenth of the full channel height). I usually add a number of sin(a*x+b*y+c*z+d) functions to the initial velocity with different values for a,b,c,d. Just random noise has a short wave length and are directly dissipated. Perhaps it is also possible to decrease the initial subgrid viscosity.

Hi, thanks for your response.

hope the i.c you are telling is like as--

do k = 0,kmax+1

do j = 0,jmax+1

do i = 0,imax+1

u(i,j,k) = 0.01 * sin(i+j*k+0.) + 1.0 ! 1.0 is the bulk velocity

v(i,j,k) = 0.01 * sin(i+j*k+1.)

w(i,j,k) = 0.01 * sin(i+j*k+2.)

p(i,j,k) = 0.0

enddo enddo enddo

Am i right. if you using anything else, could you please, send me the exact expression of that.

2nd isuue: i am colecting instantaneous signal(for every time step) of u, v, w at the channel centerline at different streamwise location.

i saw that, initially it is showing oscilational. but, as the time progress, v, w component velocity decays to 0 and u velocity increases but no oscilation observed. could you saw this type of phenomena in your simulation.

please help me.

if you want see my signal, i can mail u.

Well, it implies that the flow becomes laminar and the fluctuations disappear. Therefore, I said that you should compute the turbulent kinetic energy and watch it closely. Initially, it decreases but after some time it should increase again and fluctuate around some mean value. I guess that the initial disturbances that you impose are way to small and have a too short wave length. You should give the flow field really a kick initially otherwise it just becomes laminar.

something like u = u_mean + 0.04*sin(10*i+10*j+8*k+20)+0.03*sin(8*i+12*j+7*k+4 0)+...

and the same for the other components. Try out something!! The initial disturbance should be 10% of the bulk mean velocity or perhaps even more. If it is too much the code blows up. Then try something with a bit smaller disturbance.

Thanks tom, i will try with approach, you are telling. one more issue , i want to talk about. How you are specyfying the mean pressure gradient in the streamwise momentum equation ,that drive the flow for periodic b.c., in your code.

Are you using itarative technique. I guess a pressure gradient initially and add it to streamwise momentum equation as body force..then for a desired Re or flow rate , the pressure gradient is itaratively calculated.

are you doing the same?

For example i am giving the details how i calculate it----- --------------------------------------------------------- See, for any Re, Ubulk0 has a desired value. So, it is fixed before the code is run. for e.g--Re=4000=Ubulko*H/v So, IF you take h=1 and Ubulk0=1 v=1/4000 is the setting condition for code. That means desired flow rate is--Ubulk0=1

Now, for any time you will get Ubulk, from code .Ubulk--is the mean flow rate at outlet, calculated after copletion of wach time step.

Now update the presuure gradient as below---

p_new=p_old(1+cof((Ubulk0/Ubulk)**2-1)

First, you take a guess value of p_old, Also, Ubulk0, is known from Re. Ubulk is calculated , everytime.

And your body force term, p_new, will be updated at everytime step. when, you reach , Ubulk=Ubulk0, then after, P_new=P_old...

You just put this, P_new to your x-momentum equation.

This itarative scheme i am using.

Do you have any better idea, please tell me.

thanks.

It is more easy to impose just a constant pressure gradient. Later, when you see that the LES is working you can try something more advanced and adapt the pressure gradient so that the mean bulk velocity stays constant.

I don't know if this could help you, but i'm performing a

Ret = 180 channel flow simulation with LES in FLuent.

From previous simulations i founded that the following initial conditions is working fine:

U = -20.0*(y/H)*((y/H)-2) + 4.0*(0.5-ak)

V = 4.0*(0.5-ak)

W = 4.0*(0.5-ak)

where H is the channel half width and ak is a randomly generated number between 0 and 1.

Actually i generated it with the logistic map

a(0) = 0.5

a(k+1)= 3.891 * a(k) * ( 1 - a(k) )

because i'm not able to generate random numbers in fluent.

hope this helps

hi, Tom, Thanks for your constant advice. I have also seen a post, regarding the impose of pressure gradient in the cfd-online forum written by you.. According to that i have set my constant pressure gradient. i am explaining the same below. you please, look at the explanation and tell if i wrong.

-----------------------------------------------------

My domain is: 4piH x 2H x 2piH (dimensional)

I have non-dimensionalised by H-(half height of channel)

So my actual dimension is---4pi x 2 x 2pi

Re=U_tau x H/nu =180.(nu=viscosity)

i have taken H=1.0(clear from my non-dimensional dimension). and U_tau=1.0

So, i set nu=1/180, in my code.

As, in the code i set H=1, nu=1/180. As, i am using periodic b.c, so nowhere i can put U_tau=1.0. To, ensure U_tau=1.0, i calculate the mean pressure gradient keeping , U_tau=1.0.

so, from wall shear stress and mean-pressure balance, shows that, mean pressure gradien=1.0

And i am adding this constant pressure gradient=1.0, to my streamwise momentum equation.

So, during the computation of streamwise momentum equaation , at everycell, this added mean-pressure gradient(=1.0) is imposed .

also, i am using i.c with random perturbation.

Please,COULD YOU TELL, MY TECHNIQUE OF PROVIDING 'IMPOSE-PRESSURE GRADIENT' =1.0 IS WRONG OR RIGHT?

------------------------------------------------------

I am asking, because ...during the simulation, as you said, the mean value corresponding to the Re, will be settle down to the correct value.But, problem is that, my mean value doesnot become constatn but increasing enorsmously. for example, for Re=180, U_mean/U_tau=17.0 as, i have taken U_tau=1.0, so i should get U_mean=17.0 But, i was monitoring U_mean, at the outlet plane for every time step and saw that, it cross 17.0 and increasing and after a time of 67 it becomes 38.

Can you please, tell me where i am doing wrong in setting the problem or imposing pressure gradient?

Thanks----

Hi, Paolo thanks for the help.Could tell, what was the exact value of mean pressure gradient you appy? hope , your channel height =2.0.

could you give me the details of--

1. domain size. 2. Impose pressure gradient value. 3. Nu(viscosity) and density

thanks---

hi, Tom, Thanks for your constant advice. I have also seen a post, regarding the impose of pressure gradient in the cfd-online forum written by you.. According to that i have set my constant pressure gradient. i am explaining the same below. you please, look at the explanation and tell if i wrong.

-----------------------------------------------------

My domain is: 4piH x 2H x 2piH (dimensional)

I have non-dimensionalised by H-(half height of channel)

So my actual dimension is---4pi x 2 x 2pi

Re=U_tau x H/nu =180.(nu=viscosity)

i have taken H=1.0(clear from my non-dimensional dimension). and U_tau=1.0

So, i set nu=1/180, in my code.

As, in the code i set H=1, nu=1/180. As, i am using periodic b.c, so nowhere i can put U_tau=1.0. To, ensure U_tau=1.0, i calculate the mean pressure gradient keeping , U_tau=1.0.

so, from wall shear stress and mean-pressure balance, shows that, mean pressure gradien=1.0

And i am adding this constant pressure gradient=1.0, to my streamwise momentum equation.

So, during the computation of streamwise momentum equaation , at everycell, this added mean-pressure gradient(=1.0) is imposed .

also, i am using i.c with random perturbation.

Please,COULD YOU TELL, MY TECHNIQUE OF PROVIDING 'IMPOSE-PRESSURE GRADIENT' =1.0 IS WRONG OR RIGHT?

------------------------------------------------------

I am asking, because ...during the simulation, as you said, the mean value corresponding to the Re, will be settle down to the correct value.But, problem is that, my mean value doesnot become constatn but increasing enorsmously. for example, for Re=180, U_mean/U_tau=17.0 as, i have taken U_tau=1.0, so i should get U_mean=17.0 But, i was monitoring U_mean, at the outlet plane for every time step and saw that, it cross 17.0 and increasing and after a time of 67 it becomes 38.

Can you please, tell me where i am doing wrong in setting the problem or imposing pressure gradient?

Thanks----

My domain size is:

Lx = 4*pi*H

Ly = 2*H

Lz = 4*pi*H/3

Also i set the following values:

H = 1

rho = 1

mu = 1/Ret

dp/dx = -rho*(nu^2)*(Ret^2)/H^3 = -1

with

nu = mu / rho

My boundary conditions are periodic in x and z direction with top and bottom walls (perpendicular to the y direction).

I'm actually performing a simulation at Ret = 180 with about 266K cells

thanks Paolo---

I have 2 doubts--

1. did you take friction velocity=1.0 2. also, i hope dp/dx should be +1, not -1. Or, actually, dp/dx =+1 should be ultimately added to the right hand side of equation.

in your code if you take -dp/dx on right hand side, then its fine to take dpdx=1

did you get your result properly? could you share some time series signal or k.e with me..

thanks

I obviously have dp/dx on the right hand side of the momentum equation (i just feel more comfortable in this way) but, there should be no difference...if the flow is in the positive x direction i need a decreasing pressure in the positive x direction so dp/dx is negative to obtain such a flow

However my friction velocity is not properly 1 but a little bigger. I'm still waiting for my last 2000 time steps before starting to perform the statistics so i can't say nothing about the results but my k.e. time series is lost(parallel Fluent crashed after i inserted a wi-fi usb adapter). What i can do is to save the next iterations k.e. time series and send you a picture. Also if you have some particular need i can try to send you more pictures.

Thanks for the discussion. i have some doubt. am explaining . please take look see,

i hope to get a flow in the positive x-direction you have to add -ve pressure gradient on the r.h.s of momentum equation , but ultimately the numerical value will be added to r.h.s

because in right hand side it would be like -(-1).

because , for normal N-S eqution you see, the original pressure term looks like : -dp/dx , where dp/dx itself -ve. so, ultimate a positive pressure is added to r.h.s to drive the flow.

second question: You told that your friction velocity is little larger. there is no panel to supply friction velocity into the code as input directly. What we give directly is, taking friction velocity=1 and rho=1, height=2, we calculate viscosity from friction Reynolds no, and this is supplied as input.

do you tell, the value of friction velocity , as you obtained from simulation??

please, clarify....

do, you get any instantteneous signal?

i mean if you have u,v, w signal at channel centerline for different x-location, please send me.

thanks for the discussion...

[anzillo]

Dear Pankaj,

I hope you are doing well. Did you find out why was your flow being accelerated indefinitely?

I have the same problem with prescribing a constant pressure gradient as a body force. My flow increases in velocity.

Please let me know in case you have solved this problem.

Thank you!

Dhruv

[FMDenaro]

I suggest using the non dimensional form of the equations and setting the constant part of the pressure gradient = -1.
This way, the non dimensional velocity corresponds to V+

[anzillo]

Dear Filippo,

Many thanks for your prompt reply. I would like to know how would this pressure gradient be different from a body force?

I mean mathematically all one would do is add a source term to the RHS of the time-advancement equation, which would give the velocity field at the next time-level through du/dt = RHS (with all the other operators).

Is it that how you add this source, a body for or a constant gradient, that makes a difference? I know I am not making sense but it is weird why the methods should be different.

Thank you again for your suggestion. I will try it out quickly and let you know.

Kind regards,
Dhruv

[anzillo]

PS: I am doing an Atmospheric Boundary Layer simulation with periodic span and stream-wise boundaries and a ground with the Monin-Obukhov theory as a means to calculate the wall stress. The upper surface is an outflow boundary.

[FMDenaro]

Originally Posted by anzillo

PS: I am doing an Atmospheric Boundary Layer simulation with periodic span and stream-wise boundaries and a ground with the Monin-Obukhov theory as a means to calculate the wall stress. The upper surface is an outflow boundary.

That is different from the channel flow condition w here You have a well established driving force ... I suggest using a different condition on the upper side