Hi,I am now using LES model, and am going to run a fully-developed planar channel flow as a validation test. I read some papers, but there are still some questions about the details of the setup of the channel test. I wonder if you could give me a help. I'd appreciate it very much.

I use finite volume method to discretize the N-S equations. Pressure Poisson equation is solved to enforce the continuity and to get the pressure. The input for this problem is channel width, Reynolds number based on the friction velocity. And my questions are:

1. In some papers, the mean pressure gradient is added in the form of a source term in the momentum equation. I think that is to say decompose the pressure into a mean pressure plus a fluctuation and then do the filtering. Thus the pressure we are solving is the filtered pressure fluctuation. What is the appropriate boundary condition for it?

2. Is the mean pressure gradient fixed or changed before the flow reaches the statistically steady state? If it is changed, how does it change?

3. Why do people put some random noises into the initial velocity field? As I read from your book, the initial condition will not affect the final steady state solution.

4. Some papers say the simulation was performed with a constant mass flow rate. How to implement it, especially before the flow reaches the statistically steady state?

Thank you very much.

1. No. The pressure gradient is linear and so can be split into a sum of two parts without changing anything. The split is simply a mechanism to allow periodic conditions to be applied directly at inlet/exit for the varying part of the pressure gradient. An alternative would be to code a constant jump in pressure between inlet and exit into the implementation of the implicit pressure solvers periodic boundary conditions.

2. It depends on what conditions you are imposing on the simulation. It is usually fixed but might be varied very slightly at each iteration to enforce a force balance depending on what is being imposed to drive the flow.

3. (You have not read my book.) It does not affect the answer but it shortens the initial period when things are settling down: the transition from laminar to fully turbulent can take a long time.

4. See other thread. One simply sets up boundary conditions to maintain a constant mass flow and a force balance on the boundary. It can be useful for developing inlet conditions for a large downstream simulation which, physically, would prevent significant variations in mass flow. Alternatively one could simply scale the more usual type of simulation.

Thanks, Andy. It was a typo for 'your book'.

1. Do you apply periodic boundary condition at inlet/exit for pressure gradient? Can I apply it for the pressure itself?

4. I understand that starting from a laminar velocity field will shorten the transition time to fully-developed turbulent flow. I just don't know why to add the random noise. So I guess it is also a technique to shorten the initial period.

1. You apply periodic conditions to the fluctuating component of pressure - it is the same level at inlet and exit. The constant pressure gradient body force takes care of the decrease in pressure along the duct. The actual pressure can be recovered for plotting purposes by integrating the body force pressure gradient down the duct and adding it to the fluctuating compoent.

4. Starting from a laminar velocity field is likely to lengthen the time to reach fully developed turbulence not shorten it. By adding random noise the intention is to speed up the transition to fully developed turbulence. It is not particularly important and often achieves relatively little because uncorrelated random noise will decay away very fast. Starting from on old turbulent solution is usually more effective but the savings are not dramatic and rarely worth spending much time on.

Andy, your reply really helps a lot. Thank you.

Archie, I got your email, but the reply email was bounced back, and I don't know why. My email is wmoengr~gmail.com. (~ substituted by @). Thank you.

[niravtm007]

Hii friends
My problem is flow through river channel, I have taken a orbitary region so at exit of my geometry flow exits into river itself. so i need to know how to apply UDf at exit, as pressure must vary with P=row*g*h. my exit cross section is not uniform so what should i do please help. is it possible to apply custom field function ???? in fluent please help ASAP

[deathaldaling]

Hi,weihua,
I'm doing the validation of channel flow for the compressible LES code,and now cofused where how to and the body force in the NS equation.
As Lenormand recommanded (see fig:body-force), add body force to the left of NS equation.Averaging the momentum equation in the xy plan and integrating in the z direction,we get the Qm, and compute the first order predictor of mass flux (fig:Q). Now, I get confused how compute the driving term (fig:force),.As Lenormand said, used the extension of compressible flow of the algorithm proposed by Deschamps. I failed searching the paper.
What I want to ask is :
1. How can we get the equation of Deschamps?
2. What differences dimension and diemensionless?
3. How to set the driving force in the first time?
4. How to set the mass flux supposed to be conserved?

My email is 1375807916@qq.com
thank You!