CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Turbulent channel flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   August 15, 2007, 05:35
Default hi its me again. maybe someone
  #1
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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?
roberthino is offline   Reply With Quote

Old   August 15, 2007, 05:57
Default Hi, To start with, you need
  #2
Member
 
Ola Widlund
Join Date: Mar 2009
Location: Sweden
Posts: 87
Rep Power: 8
olwi is on a distinguished road
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 is offline   Reply With Quote

Old   August 15, 2007, 06:00
Default Forgot to say: Since you want
  #3
Member
 
Ola Widlund
Join Date: Mar 2009
Location: Sweden
Posts: 87
Rep Power: 8
olwi is on a distinguished road
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
olwi is offline   Reply With Quote

Old   August 15, 2007, 06:00
Default thank you. well i thought this
  #4
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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
roberthino is offline   Reply With Quote

Old   August 15, 2007, 07:49
Default Some alternatives: 1. Maybe
  #5
Member
 
Ola Widlund
Join Date: Mar 2009
Location: Sweden
Posts: 87
Rep Power: 8
olwi is on a distinguished road
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
olwi is offline   Reply With Quote

Old   August 15, 2007, 08:35
Default well i see. what about doing a
  #6
Member
 
robert maduta
Join Date: Mar 2009
Posts: 33
Rep Power: 8
roberthino is on a distinguished road
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
roberthino is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
LES In Turbulent in channel flow pankaj saha Main CFD Forum 18 November 20, 2014 06:49
Turbulent channel flow by LES Paul Main CFD Forum 14 July 6, 2009 04:02
LES In Turbulent in channel flow pankaj saha Main CFD Forum 8 April 15, 2009 11:34
Bc for turbulent channel flow roberthino OpenFOAM Running, Solving & CFD 0 August 13, 2007 08:12
turbulent channel flow profile otto mierka Main CFD Forum 3 August 23, 2005 11:56


All times are GMT -4. The time now is 20:26.