CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Channel Flow pisoFoam SA IDDES Re=4560 (http://www.cfd-online.com/Forums/openfoam-solving/114544-channel-flow-pisofoam-sa-iddes-re-4560-a.html)

ingcorra March 13, 2013 04:56

Channel Flow pisoFoam SA IDDES Re=4560
 
Im trying to get a fully developed turbulent flow in a channel with a mapped inlet boundary, periodic sides and fixed upper and lower walls. The only way to get some turbulence is to set nuTilda = 0 at inlet, which as far as I know is an ideal condition but then I get zero iterations for nuTilda (so the turbulence model is doing nothing). Any other value different from zero causes the complete dissipation of the turbulence and the flow to be laminar. Is this due to the low Reynolds number? Is it correct to keep nutilda=0 at inlet and have no iterations?

I have the following bundary conditions for nuTilda and nuSgs:

nuTilda

inlet, upper and lower walls: fixedValue 0
outlet: zeroGradient
sides = periodic

nuSgs

sides = periodic
everywhere except at the sides: zeroGradient

Lieven March 13, 2013 05:30

Hi Ingcorra,

If you want to use pisoFoam, you should modify the solver a bit to include a pressure gradient or fixed mass flow rate. Else your flow will simply slow down till there is no flow at all. But you would simply end up with the channelFoam solver. So my advice, start from the latter (is basically an extended version of pisoFoam, but only for LES models).

Cheers,

L

ingcorra March 13, 2013 05:37

Hi Lieven,

thanks for your reply. I forgot to mention that the inlet condition for the U is mapped and has an average value that provides Re=4560, so the flow is not definitely slowing down. Im using it to validate a modified pisoFoam solver (which includes a scalar transport equation) along with the IDDES model with DNS data so I prefer not to use the channelFoam solver.

Lieven March 13, 2013 06:37

Ok, that changes things :D

Why do you map only the velocity field?
Seems to me that you should do the same with the other fields like nuSgs. You can turn of the averaging for these fields because once the steady condition is reached, the averagingfactor of the U-field should be close to 1.

cheers,

Lieven

ingcorra March 13, 2013 07:19

I mapped nuSgs and nuTilda too (without no average value of course) but I still get zero iterations :confused:

ingcorra March 22, 2013 03:08

I solved by choosing a different initial condition for nuTilda (near to nu). It just converges to a steady value very slow, thanks for the help

AA29 April 5, 2013 13:19

Hi ingcorra,

I am facing the same problem. I increased the Re=12000, even then the flow eventually becomes laminar.Did you find a solution to this problem?:confused:

Any help will be highly appreciated.

AA29 April 5, 2013 13:32

And i forgot to mention that i am using channelfoam intead of PISOfoam to simulate a fully developed turbulent flow.

ingcorra April 5, 2013 15:02

You have to provide a correct initial value for nuTilda and nuSgs. There are formulas to calculate it but I guess they're suitable only for external aerodynamics. You could use an initial condition calculated with another turbulence model or just make nuSgs=nuTilda=nu (I assume you already know how to set up the boudary conditions). Let it run until you have an eventually laminar steady flow and check if you have somewhat stable residuals for nuTilda, then add some randomisation to the velocity field and it should develope a nice turbulence ;)

huangxianbei March 3, 2014 21:37

Quote:

Originally Posted by Lieven (Post 413631)
Ok, that changes things :D

Why do you map only the velocity field?
Seems to me that you should do the same with the other fields like nuSgs. You can turn of the averaging for these fields because once the steady condition is reached, the averagingfactor of the U-field should be close to 1.

cheers,

Lieven

Hi.Lieven
I faced a problem of the convergence when using the icoFoam including pressure gradient. Both the fixed pressure gradient and fixed mass flow rate are performed, however, when I monitor the pressure gradient in the mass flow rate case, the pressure gradient decreases along time steadily, that means delta(grad(p))=const in the same time step change. Also, in the case of fixed pressure gradient, the velocity at the centerline increase steadily as the pressure gradient in mass flow rate case. I don't know why this happens.

vut March 13, 2014 10:58

Hi all,

I use OpenFoam for a couple of time (several weeks only). Please be gentle and slow :)

I am interested in your topic. My task is to simulate a turbulent flow inside an injector.

The solver pisoFoam seems to be suitable for my case study.

Your experiences are greatly appreciated for my following questions:

* Do you have idea about the boundary condition for nuSgs at the symmetry plane.

* How can the lastest solutions of RANS (computed by simpleFoam) be imported as initial conditions for pisoFoam?

All your ideas are wellcome.

Thanks in advance,

VUT


All times are GMT -4. The time now is 09:12.