Hi all:

I use LES to simulate compressible turbulent

channle flow. In viscous terms, I used centeral difference

scheme. In non viscous terms, I used Roe with MUSCL

scheme and add preconditioning. In boundary condition, I

use periodic condition in streamwise and spanwise direction

and add pressure gradient to drive the flow. My problem is

the flow is always become laminar or the perturbation is

become very small. Is the initial filed is wrong or my

scheme is wrong ?

Hi Ricklee,

what about your CFL number? What dt r u using? It's because there is a paper from choi and moin where they said that the flow got laminar when the dt was too large, killing all the fluctuations...

Try to reduce your CFL number or dt...

See ya...

Thanks for your reply, Newton:

Actually, I set dt very small, Even I add

preconditioning in Roe scheme. The CFL number in

preconditioning is U*dt/dx or (U+C)*dt/dx where

C is the son speed. If the CFL is U*dt/dx, my CFL is

0.3. If the CFL is (U+C)*dt/dx, the CFD is 78. Can you

give me some suggestion?

Hi,

Roe-MUSCL is pretty dissipative to be used in the LES approach. Upwind schemes are usually used in the MILES approach (without SGS model).

1) Do you use any SGS model ? 2) What is the order of your MUSCL reconstruction ? 3) Have you tried a finer mesh for the same case ? 4) Do you have any other scheme to compare them ?

Regards

Thanks for your reply, buch:

I read you question and the answer is

1) I used smagorinsky model and add damping term to

keep the C near the wall is close to zero

2) My MUSCL scheme is 3 order

3) I try very finer grid with y+ < 3 in the first grid

4) Can you give me some suggestion about what scheme

I can use

Thank you.

You're welcome You may try to :

1) turn the SGS off. Does it blow up ? 2) use 5th ou higher order MUSCL if it is possible ; 3) verify your MUSCL version does not include any unwanted limiting process (you know, TVD stuff, used for compressible cases); 4) change your base scheme : if you already have a Roe scheme, coding an FVS scheme like the AUSM+-up should not be that difficult. Otherwise you may try many classical centered schemes, but their implementation might need more work given your base scheme ... 5) how do you advance in time ?

Regards

Buch

Thanks for your reply, buch:

1) If I turn off SGS, it also become laminar.

4) Can AUSM+-up scheme also add preconditioning to

make the compressible code to simulate very

low Mach number ?

5) I add dual time stepping and used LUSGS implicit

time scheme.

Dual time stepping can be used for LES, but I do not think it is the best approach. DTS allows you to use large time steps compared to other classical approaches. But, physically the use of large dt will smooth the small unsteadinesses. And if you decrease dt, the necessary sub-iteration process will make the overall DTS process cost prohibitive !

So, you may try another approach for your advance in time. Classical explicit RK methods for example.

And for the AUSM+-up, sure you can add a preconditionning technique. Liou in his paper uses one.

Regards

Thanks for your reply, buch:

I try to solve the problem alomost for half year.

Thanks for you give me so much suggestion in one days.

Because preconditioning is add in original time terms,

I have to add DTS in original N-S. If not, the time terms

is change and the N-S eqs is wrong. How to use Classical

explicit RK methods and make the time term is reasonable?

Hum, for this specific aspect, Il will not help you much. I am used to conduct compressible simulations, and I have no real idea of how RK+low Mach preconditonning is achievable (if it is). Sorry.

However, if you turn off the preconditioning and increase the Mach number, do you still have the same damping problem ?

Thanks for your reply, buch:

I never do that in my code. I read a AIAA paer

writed by Trong T. Bui he used the same method with me but

in Roe scheme he make some change.

F = 0.5*(F_L+F_R)+0.5*eplison*abs(A)*(U_R-U_L)

In general, eplison = 1 and his eplison is < 0.01.

If I use the eplison in my code, it will be divergence.

Try to send him an email ... Sometimes there are some typographic errors in papers, and you will gain a lot of time asking him directly instead of trying by yourself, especially if the published formula is wrong

What kind of initial disturbances do you impose and how large are these?

Hello, tom:

I make a fully developed turbulent profile and add

20% disturbance in velocity. Because I don't know how

to create a data with turbulent correlation. But I think

just a lot of steps, it will appear right correlation in

computational domain.

I was wondering if you use just random disturbances. If these disturbances have a very short length scale they are quickly dissipated. Then it is better to use random cos/sin disturbances with a quite long length scale. These are not as quickly dissipated.

Thanks for your suggestion,Tom:

Actually, I have try to done the cos/sin disturbances

before.

http://www.cfd-online.com/Forum/main...cgi?read=45389

But I did not know the meaning about the symbol.

If could, can you give me some reference about cos/sin

disturbances with a quite long length scale?

Thank you.

The trigonometric functions sine and cosine. In fortran these are the functions sin() and cos().

Hello, tom:

If I add white Gaussian noise distribution,

did you think the length scale is long enough?

I'm not exactly sure what you mean. If you add a different random perturbation at every grid cell the length scale is very short. In this case the disturbances will be dissipated very quickly. Better is to use disturbances of the kind mentioned before.