CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Atmospheric Boundary Layer high turbulent flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 19, 2014, 05:03
Default Atmospheric Boundary Layer high turbulent flow
  #1
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Hi everybody,

I'm trying to simulate an atmospheric boundary layer (ABL) flow around an inclined flat plate near the ground. I'm not developping the whole boundary layer but using velocity, k and epsilon profiles at the inlet with UDF's (there's no option to use turbulence intensity and turbulent length scale UDFs).

I've used a logaritmic profile for velocity:

u(h)=Uref*K*log(h/h0)

Uref=reference velocity (10 m/s)
K=constant (0.1866)
h0=roughness height (0.03 m)

I defined the turbulence intensity and turbulent length scale (TLS) profiles to get the k and epsilon profiles:

TI(h)=1/log(h/h0)

TLS(h)=Lt*(h/ht)^alpha

alpha=constant (0.4947)
ht=reference heigth (200 m)
Lt=reference TLS (300 m)

k=(3/2)*(Uref*TI)^2

TI from former TI profile equation

epsilon=C_mu^(3/4)*k^(3/2)/TLS

TLS from former TLS profile equation
C_mu=constant

Below h_min=1.5 m all profiles have a constant value equal to u(h_min),k(h_min) and epsilon(h_min).

I've initialized from the inlet but the issue is that with these profiles I get turbulent viscosity limitation from the very beginning. Even if I change the TVR limit to 10e15 limitations is reached very soon.

Does anybody have experience simulating atmospheric boundary layers?
Any advice on how to avoid this limitation?
Is it a matter of mesh density? Cause I cannot go beyond my current 2 million elements mesh... And I've seen some meshes in literature that are not very dense.

I post a picture with all the profiles involved in the simulation and some mesh screenshots.
Attached Images
File Type: jpg mesh_cut_plane.jpg (90.3 KB, 10 views)
File Type: jpg mesh_cut_plane_iso.jpg (92.0 KB, 9 views)
File Type: jpg mesh_plate.jpg (85.1 KB, 9 views)
File Type: jpg profiles.jpg (57.0 KB, 10 views)

Last edited by Bollonga; February 20, 2014 at 06:14.
Bollonga is offline   Reply With Quote

Old   April 16, 2014, 12:49
Default
  #2
New Member
 
Marco Leonardelli Lovatto
Join Date: Nov 2011
Posts: 9
Rep Power: 5
marcolovatto is on a distinguished road
Hello Francisco!

I'm also beginning on ABL, let's learn together?

The order of magnitude of your TVR is too high... 1e8?? Is it an input or an output of TI and TLS input?

It seems you're using ICEM for meshing... what is your solver?

Last edited by marcolovatto; April 16, 2014 at 12:56. Reason: question added
marcolovatto is offline   Reply With Quote

Old   May 30, 2014, 08:03
Default
  #3
Senior Member
 
Francisco
Join Date: Mar 2012
Location: Spain
Posts: 270
Rep Power: 5
Bollonga is on a distinguished road
Hi Marco, sorry for a too late answer.

Quote:
Originally Posted by marcolovatto View Post
The order of magnitude of your TVR is too high... 1e8?? Is it an input or an output of TI and TLS input?
I've read that TVR of 1e8 or higher are usual in ABL flows, as there is a lot of turbulence near the ground.
TVR is derived from TI and TLS, so TVR can be considered as an output of TI and TLS or k and epsilon.

I've solved my problem by applying different boundary conditions (k and epsilon) to the ones suggested by the Eurocode (TI and TLS and then transformed to k and epsilon with Fluent users guide formulae). I've also refined the mesh specially near the ground, to get the high gradient present in the layers near the ground.

I've followed the boundary conditions form this reference:

Richards and Hoxey 1993: Appropriate boundary conditions for computational wind engineering models using the k-ϵ turbulence model

http://www.sciencedirect.com/science...67610593901247

In the next reference there's a simple example I've run to check the proposed mesh, it uses the former Richards and Hoxey BC:

Hargreves and Wright:On the use of the k ε model in commercial CFD software to model the neutral atmospheric boundary layer

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

Quote:
Originally Posted by marcolovatto View Post
It seems you're using ICEM for meshing... what is your solver?
I'm using Fluent v14

How are you going with your ABL simulation?

Hope this helps!
Bollonga is offline   Reply With Quote

Reply

Tags
abl, atmospheric bl, high turbulent flow

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
Wind turbine simulation Saturn CFX 34 October 16, 2014 06:27
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 08:00
Automobile aero ground boundary layer OR simpleFoam/GAMG and high aspect ratio cells kyle OpenFOAM Running, Solving & CFD 4 January 4, 2011 12:17
[GAMBIT] 3D Boundary Layer Laminar and Turbulent meshing Harald D ANSYS Meshing & Geometry 1 July 7, 2009 07:20
How to generate a atmospheric boundary layer Morten Andersen CFX 3 January 16, 2007 07:48


All times are GMT -4. The time now is 11:15.