CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   help with boundary conditions (http://www.cfd-online.com/Forums/openfoam-solving/96075-help-boundary-conditions.html)

 dshawul January 11, 2012 14:57

help with boundary conditions

2 Attachment(s)
I am trying to do ABL simulation using OF on an open area. It is a simple case where a uniform velocity is applied at the inlet and a uniform pressure at the outlet. I am getting high values of pressure at the bottom of the inlet (about 400pa as shown in the figure). The more I refine the mesh the larger its value is, so I am wondering if my boundary conditions are correct or not ? I would really really appreciate your help in solving this problem. I have attached the case file with the boundary conditions I am using.
Thank you

 fcollonv January 12, 2012 07:15

Hello Daniel,

Your test case looks very similar to a turbulent flat plate case (I don't know what ABL means - abbreviation are not recommended...). If so, here is a known test case that could be useful: http://www.grc.nasa.gov/WWW/wind/valid/fpturb/fpturb.html
You will see that for incompressible flow, the first point of the plate is a singularity (hence your high value there that get higher but more localized when the mesh is finer). It's therefore better to put the inlet ahead of the interesting section (see nasa test case)

I have also some questions:
* why are you using a 3D mesh, when your case is obviously 2D ??
* why are you setting the pressure to 1 at the outlet? The value of the pressure in incompressible case is relative, so the reference is usually 0 (as set in your system/fvSolution::SIMPLE). And consequently the outlet is usually set to that reference.

Frederic

 dshawul January 12, 2012 10:31

Dear Frederic
Thank you very much! That was really helpful. ABL = atmospheric boundary layer flow. I didn't know that p would be singular at bottom of the inlet. As in the flat plate case, I have an internal boundary layer developed in my test case too. I want to avoid that by applying a log-law inlet velocity profile. In which case the profile should come out intact at the other end too. I wanted to try uniform profile before doing that which caused this "problem".

I have corrected the value of p to 0 at the outlet and will be using 2D mesh for my next tests.

I have other questions if you don't mind:

My y+ values are very big and I can not bring it down by using a fine mesh close to the wall because of another constraint that yp > Ks. Ks is the equivalent sand grain roughness for a rough wall as used in nutRoughWall of OF. I will be using rough walls later which could have ks values as high as 15m. What does OF do when y+~=20000 , does it still apply log-law ?

thanks again
Daniel

 fcollonv January 16, 2012 06:15

Law of the wall and big y+

Hey

Quote:
 Originally Posted by dshawul (Post 339041) My y+ values are very big and I can not bring it down by using a fine mesh close to the wall because of another constraint that yp > Ks. Ks is the equivalent sand grain roughness for a rough wall as used in nutRoughWall of OF. I will be using rough walls later which could have ks values as high as 15m. What does OF do when y+~=20000 , does it still apply log-law ?
As far as I know, it will apply the log-law for any y+ bigger than the y+_laminar. But it's up to you if you want to implement something different or not using it...

Cheers,

Fred

 All times are GMT -4. The time now is 20:04.