CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Turbulent channel flow (https://www.cfd-online.com/Forums/openfoam-solving/59503-turbulent-channel-flow.html)

 roberthino August 15, 2007 05:35

hi its me again. maybe someone

hi its me again. maybe someone can help me now. i am tryin g to do a steady state analysis of turbulent channel flow with rng-k-e-model. my channel has the height and width of 0.2 meters and the length of 3 meters. i am doing a 2-D analysis with 50 gridpints in height direction and 100 in streamwise direction. after 10000 iterations i get godd profiles for epsilon, the streamwise velocity and the pressure. the profile for k is still wrong (highest value in the midle of the channel. the values for all my parameters are all totally wrong (for example the velocity is around 0.0003 and the pressure 5.0e-13 etc). as boundary condition i chose cyclic for inlet-outlet and wall-function for the walls and empty for the third dimension. i set my viscosity to 8.0e-4. what am i doing wrong? why are the values so crazy? do i simply have to do a lot more iterations?

 olwi August 15, 2007 05:57

Hi,

To start with, you need a contstant streamwise pressure gradient. Otherwise you wont have any flow. I think you can set zero-gradient BC:s on the patches upstream and downstream for all variables, but you need to add the pressure gradient as a constant source term in the streamwise momentum equation.

Once that works, I would try using an AMG solver for both momentum and pressure, because this rather particular case will converge very slowly (the solution between the walls will propagate only by diffusion, since convection is only parallel to the walls). I think OF 1.4 has an AMG solver that works for momentum as well (OF 1.3 has not, though).

/Ola

 olwi August 15, 2007 06:00

Forgot to say: Since you want

Forgot to say: Since you want a fully developed flow, you need only one or two cells in the streamwise direction...

This flow may appear trivial, but it converges a lot slower than problems where convection plays a more important role in the propagation of information in the domain.

/Ola

 roberthino August 15, 2007 06:00

thank you. well i thought this

thank you. well i thought this is already implemented for simple foam....hm....maybe you can explain me how to add the constant source term in the streamwise momentum equation.....do i have to edit a file? and if, then which one?
sorry but i am really new, and i thought that with cyclic boundary condition he is doing all by its one with iterations

 olwi August 15, 2007 07:49

Some alternatives: 1. Maybe

Some alternatives:

1. Maybe the solver boundaryFoam does what you want. I think it's used to generate realistic inlet bc:s for other solvers, but maybe the way it's done can be confusing to you.

2. To get a constant pressure gradient in there, you need to make your own copy of a solver like simpleFoam or turbFoam, change its name, add the source, and then compile your new solver. See the guidelines for instructions and information. The magnitude of the pressure gradient can be read at runtime, if you code your solver to read the value from one of the case dictionaries. See the source code of createFields.H to see how that is done for other parameters.

3. In principle you can take any of the turbFoam or simpleFoam solvers, and use fixed-value BC:s on pressure upstream and downstream. Make a small difference in relative pressure between inlet and outlet. You need to make a good estimate how big the pressure difference should be, to give you a reasonable velocity.

In any case, you need to start looking at the source code for the solvers, and understand what equations are solved, and how. You will have to edit more than one file, for sure. No point in telling you which ones, you need to get your hands dirty for this to work for you...

Good luck!

/Ola

 roberthino August 15, 2007 08:35

well i see. what about doing a

well i see. what about doing all the stuff 1-D with simple foam and to put also empty for in let and outlet because of fully developed flow? another thing: what about taking inlet and outlet BC and to take a very long channel so the perturbations because of the not so good BC can shrink? What a pitty that boundary foam is not working. openfoam cant read it

 All times are GMT -4. The time now is 18:32.