CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Pre-Processing

value of k for atmospheric wind

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 24, 2021, 15:10
Default value of k for atmospheric wind
  #1
New Member
 
Adrian Main
Join Date: Jun 2021
Location: UK
Posts: 2
Rep Power: 0
AdrianMm is on a distinguished road
Hello everyone. I am quite new to OpenFOAM and I would like to know if I could please get the advise from any of you related to the next topic:

A bit of context: I am running a Atmospheric Wind simulation, within the field of civil engineering, sort of what we do with wind tunnels tests. I have a structure imported from STL format, in the middle of a quadrilateral blockMesh and I am subjecting it to a wind. I have successfully snapped the geometry with SnappyHexMesh. I want to obtain surface pressures and pressure coefficients on my object (a building).

I am using simpleFoam to solve the model with realizableKE turbulent model. The boundary conditions are quite critical. I have used the ones from here, based on the paper from Hargreaves and Wright (2007):

https://develop.openfoam.com/Develop...ht_2007/0.orig

I have implemented these boundary conditions. Are they correct/advisable for my study? I had to cancel the “Top” wall shear since it was making my model to diverge but I don’t think this is critical. Is it?

I am experiencing some troubles to define the internalField value for “k”, in the “k” input file. My results are super sensitive to this input value and completely dependent on it (despite I thought this was just an initial setup and then the analysis is to work its way towards the right k it needs…). But no, it is critical to get this number right. From the equation k = friction velocity^2 / Cmu^0.5 I get a big number (k=8.57 obtained with rho=1.184, kappa=0.42, z0=0.03, zref=10 and Uref=22.2) leading to what I deem unrealistically huge vortices and very bad convergence. By trial and error I’ve found that the results I consider about-right are for an internalField close to k=0.1.

Can anyone make sense of all this? Which is the “k” I should be using (and why)?

Many thanks for your help. Adrian
AdrianMm is offline   Reply With Quote

Old   June 25, 2021, 04:45
Default
  #2
Senior Member
 
piu58's Avatar
 
Uwe Pilz
Join Date: Feb 2017
Location: Leipzig, Germany
Posts: 727
Rep Power: 13
piu58 is on a distinguished road
There is something wrong if your results depends on initial k in a strong way. The simulation should find the adequate value by itself. An unfavorable starting value may lead to an exploding simulation. But if that not happens, the final result should not depend on the starting point.

I assume that something is wrong with you model. A hint for this is that you had to remove b.c. for the top.

Some proposals:
1) build a simple geometry with the same physics (and all boundary conditions) and look what happens. Blockmesh should be sufficient for that.
May be, your model is unphysical.
BTW, you get a realistic value for k from this.

2) run checkmesh. Look first at non-orthogonality which should be less than 50 or 60 for rather physical complicated models.
Look if there are elements with large non orthogonality in the near of the areas where you need the solution.
Improve the mesh. If that is not possible, rather simplify the geometry instead of using a bad mesh.

3) Use robust methods for discretization and solving instead of very accurate ones. If you get decent results with that you may proceed with more accurate ones.
__________________
Uwe Pilz
--
Die der Hauptbewegung überlagerte Schwankungsbewegung ist in ihren Einzelheiten so hoffnungslos kompliziert, daß ihre theoretische Berechnung aussichtslos erscheint. (Hermann Schlichting, 1950)
piu58 is offline   Reply With Quote

Old   June 25, 2021, 10:02
Default
  #3
Senior Member
 
Join Date: Apr 2020
Location: UK
Posts: 454
Rep Power: 11
Tobermory will become famous soon enough
The Hargreaves and Wright paper applies what are called "Surface Layer Approximation" profiles to the lower part of the ABL. These are essentially the same as a constant stress approximation, and are a high Re# asymptotic state for the log law region. In other words, they are a basic approximation for the lower 50m or so of the ABL, and are a pretty poor representation of anything above this.

For some reason, this H&W paper has been taken as a manual, and these boundary conditions seem to be being used widely across the CWE industry, even by consultancies who are also doing wind tunnel modelling (who should know that the idea of a constant k profile across the ABL is nonsense!).

A more physical k profile would have the values decaying with height; a linear decay usually gives a good fit to wind tunnel data (ignoring Coriolis effects and wind shear).

Once you have your profile, do as piu58 suggests - pass it through an empty (2d) domain, and see if your profiles develop. If they do develop significantly, then your inlet BCs are not in balance with your ground BC, so check the details again.
Tobermory is offline   Reply With Quote

Reply

Tags
atmboundarylayer, realizableke

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Pitsco Airtech 40ic wind tunnel manual & software needed Q-Prof Main CFD Forum 2 May 15, 2019 13:26
simulating wind shear profile for a wind turbine--> How??? mohammad CFX 14 August 25, 2014 09:09
simulating wind shear profile for a wind turbine--> How??? mohammad FLUENT 0 April 14, 2012 23:54
Simulate the wind profile on a wind turbine---> HOW ???? mohammad Main CFD Forum 0 April 13, 2012 08:16
Simulate the wind profile on a wind turbine---> HOW ???? mohammad Main CFD Forum 0 April 13, 2012 08:07


All times are GMT -4. The time now is 14:12.