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

Flat Terrain ABL problem

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

Like Tree2Likes
  • 1 Post By Lieven
  • 1 Post By Lieven

Reply
 
LinkBack Thread Tools Display Modes
Old   April 23, 2013, 07:47
Default Flat Terrain ABL problem
  #1
Member
 
Davide
Join Date: Dec 2012
Posts: 32
Rep Power: 4
Davide_sd is on a distinguished road
Hi all,
i'm new to openFoam; i have read the userguide and i've done the tutorials.

I have started with a small simulation of a 2D flat terrain; i've managed to setup the Atmospheric Boundary Layer inlet condition. Basically i have modified the simpleFoam/turbineSiting tutorial, and i've reduced the turbulentKE because my simulation domain is small (1.65 m long, 0.24 m height).

I'm puzzled about the results; as you can see in the picture, i've plotted the velocity profile at the inlet (dark red), mid section (green), outlet (cyan). In the horizontal axis there is velocity magnitude [m/s], in the vertical axis there is Height [m].
The velocity profile is somehow modified along the terrain, and i'm pretty sure it is wrong. What can i do to correct this issue?

PS: In this link you can find the simulation... it is too big to upload it in the attachment.
Attached Images
File Type: jpg Schermata del 2013-04-23 09:02:47.jpg (25.8 KB, 41 views)
Davide_sd is offline   Reply With Quote

Old   April 25, 2013, 03:08
Default
  #2
Member
 
Davide
Join Date: Dec 2012
Posts: 32
Rep Power: 4
Davide_sd is on a distinguished road
please, anyone can help me?
Davide_sd is offline   Reply With Quote

Old   April 30, 2013, 11:29
Default
  #3
New Member
 
ze
Join Date: Jan 2013
Posts: 1
Rep Power: 0
studenric is on a distinguished road
hi

Iíve just seen your thread and I've checked your case. I'm not sure, because i'm also new to openFoam, but i think your top conditions shouldn't be those of a symmetry plane...they should be equal to the inlet conditions...but that's my opinion and like Iíve said, Iím also new to openFoam.

best regards
studenric is offline   Reply With Quote

Old   April 30, 2013, 16:10
Default
  #4
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
Dear Davide,

What you see in the graph is the result of two things:
1. The log-profile is only the solution to the equations for a particular set of BC. E.g. at the top of the BC you should set a fixed shear stress and not a symmetry plane.
2. (the main reason) At ground level, the gradient of the velocity behaves strongly non-linear. When you apply e.g. linear interpolation to the velocity field, you will make a large numerical error. At higher altitudes, the gradient is smaller and this is less of a problem. Hence, the profile is mainly distorted at ground level.

I would recommend you to read the following papers. The first one discusses (1) and the second one (2). If you implement the content of both papers in OF and rerun your simulation, you will get a perfectly logarithmic velocity profile.

http://www.sciencedirect.com/science...6761050600136X

http://onlinelibrary.wiley.com/doi/1...nticated=false

Enjoy ;-)


Lieven
Davide_sd likes this.
Lieven is offline   Reply With Quote

Old   May 6, 2013, 08:52
Default
  #5
Member
 
Davide
Join Date: Dec 2012
Posts: 32
Rep Power: 4
Davide_sd is on a distinguished road
Thank you guys.
@Lieven, those are really interesting papers, thank you!!!
Davide_sd is offline   Reply With Quote

Old   August 6, 2013, 09:11
Default
  #6
Senior Member
 
EloÔse
Join Date: Jul 2012
Location: Trondheim, Norway
Posts: 103
Rep Power: 5
Eloise is on a distinguished road
Quote:
Originally Posted by Lieven View Post
1. The log-profile is only the solution to the equations for a particular set of BC. E.g. at the top of the BC you should set a fixed shear stress and not a symmetry plane.
Hello Lieven,

Could you explain how do you implement a fixed shear stress on the top boundary condition in OpenFoam? Is is sufficient to impose a constant velocity (Ux equal to the inlet velocity at corresponding height)?

Regards,
EloÔse
Eloise is offline   Reply With Quote

Old   August 6, 2013, 09:15
Default
  #7
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
Hi EloÔse,

The fixedShearStress boundary condition is available in OF ;-).

Imposing the velocity might work, and is physically "correct" in case of an open field with perfect numerics. But as soon as you have objects in your domain and numerical errors (due to discretization), it is not the right way to go.

Cheers,

Lieven
luismsc likes this.
Lieven 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
conduction problem venkataramana OpenFOAM 3 December 1, 2013 08:30
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Problem Importing Geometry ProE to CFX fatb0y CFX 3 January 14, 2012 20:42
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13


All times are GMT -4. The time now is 13:38.