CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   Boundary Conditions for Atmospheric flow (https://www.cfd-online.com/Forums/openfoam-pre-processing/119959-boundary-conditions-atmospheric-flow.html)

oystein_myrmo June 27, 2013 10:35

Boundary Conditions for Atmospheric flow
 
I am fairly new to OpenFOAM, so please bear with me. I am looking to set up an atmospheric flow around an offshore platform. The inlet wind conditions can be set by using the atmBoundaryLayerInletVelocity BC. I am wondering about the other BCs, however. What are the best BCs for the sides, top, outlet and bottom of the domain? The bottom of the domain is assumed to be water (flat). Also, what are the best BCs for the structure itself? My physical variables are velocity, pressure, k and epsilon.

So far I am thinking the following, please correct me where I am wrong and fill in where I am wondering:

Velocity:
- Inlet: atmBoundaryLayerInletVelocity
- Outlet: ???
- Sides: ???
- Top: slip ???
- Water: fixedValue 0
- Walls: fixedValue 0

Pressure:
- Inlet: inletOutlet
- Outlet: outletInlet
- Sides: ???
- Top: ???
- Water: zeroGradient
- Walls: zeroGradient

k and epsilon:
- Same as for velocity?

Any comments are highly appreciated! Are there any good references for descriptions of the BCs other than Doxygen?

oystein_myrmo July 9, 2013 03:40

I will give you my current take on this. Please correct me if I'm wrong.

Velocity:
- internalField uniform (Ux Uy Uz)
- Inlet: atmBoundaryLayerInletVelocity
- Outlet: inletOutlet (inletValue uniform (0 0 0) )
- Sides: slip
- Top: slip
- Water: fixedValue (value uniform (0 0 0) )
- Walls: fixedValue (value uniform (0 0 0) )

Pressure:
- internalField uniform 0
- Inlet: zeroGradient
- Outlet: fixedValue (value $internalField)
- Sides: slip
- Top: slip
- Water: zeroGradient
- Walls: zeroGradient

k:
- internalField uniform ( (3/2)*(U*I)^2 as given here: http://www.cfd-online.com/Wiki/Turbu...ary_conditions )
- Inlet: fixedValue (value $internalField)
- Outlet: inletOutlet (inletValue uniform 0)
- Sides: slip
- Top: slip
- Water: zeroGradient
- Walls: kqRWallFunction (value $internalField)

epsilon:
- internalField uniform ( C_mu^(3/4) * k^(3/2) / L as given here: http://www.cfd-online.com/Wiki/Turbu...ary_conditions )
- Inlet: fixedValue (value $internalField)
- Outlet: inletOutlet (inletValue uniform 0)
- Sides: slip
- Top: slip
- Water: zeroGradient
- Walls: epsilonWallFunction (value $internalField)

I am a bit uncertain of whether I should use inletValue $internalField or uniform 0 for k and epsilon. Does anybody have any recommendations for this? Should the water be treated by wall functions rather than zeroGradients? The scale of the cells at the water level is likely to be around 1 m.

Niru July 29, 2013 10:29

Boundary conditions
 
hi


Reg the boundary conditions. Offshore platforms and atmosphere surrounding it is an open environment and flows in open environment are called external flows.
I dont know about open foam , but in CF, we can use the Open boundary conditions for side walls and top of atmosphere. A opening BC will allow velocity to go inside and outside the domain reflecting the actual wind in atmosphere. Usually pressure values are not known in external flows. You have to run a steady state run for few iterations using outflow pressure conditions (usually 0 pressure difference) , find the pressure values from steady state run and use the values for transient run. The offshore platform as such is considered as a rigid body in the simulation.

BTW
Your work on "Numerical modeling of pool spreading,
heat transfer and evaporation in
liquefied natural gas (LNG)" was good. I am assuming that you wrote this thesis.

Lieven July 29, 2013 10:52

Hi all,

Although it seems like a very simple problem to set the boundary conditions, it is actually quite tricky. Have a look at the following papers for more information:

* Richards, P., & Hoxey, R. (1993). Appropriate boundary conditions for computational wind engineering models using the k-ϵ turbulence model. Journal of Wind Engineering and Industrial Aerodynamics, 47, 145–153.
* Blocken, B., Stathopoulos, T., & Carmeliet, J. (2007). CFD simulation of the atmospheric boundary layer: wall function problems. Atmospheric Environment, 41(2), 238–252. doi:10.1016/j.atmosenv.2006.08.019
* Sumner, J., & Masson, C. (2011). k- epsilon simulations of the neutral atmospheric boundary layer: analysis and correction of discretization errors on practical grids. International Journal for Numerical Methods in Fluids. doi:10.1002/fld

It is for example very tempting to set the slip condition at the top of the domain but this will introduce a modeling error which, depending on the extent of the domain, can become non-negligible...

Cheers,

Lieven

oystein_myrmo August 4, 2013 07:55

Quote:

Originally Posted by Niru (Post 442604)
Reg the boundary conditions. Offshore platforms and atmosphere surrounding it is an open environment and flows in open environment are called external flows.
I dont know about open foam , but in CF, we can use the Open boundary conditions for side walls and top of atmosphere. A opening BC will allow velocity to go inside and outside the domain reflecting the actual wind in atmosphere. Usually pressure values are not known in external flows. You have to run a steady state run for few iterations using outflow pressure conditions (usually 0 pressure difference) , find the pressure values from steady state run and use the values for transient run. The offshore platform as such is considered as a rigid body in the simulation.

Thank you for your comments. This is the kind of BCs I am looking for, but I cannot really find a suitable one in the source code. I found one called freeStream though, described as This boundary condition provides a free-stream condition. It is a 'mixed' condition derived from the inletOutlet condition, whereby the mode of operation switches between fixed (free stream) value and zero gradient based on the sign of the flux. I am not sure if this will be correct either, since this BC is derived from an outlet BC. I'll look at bit more into it.

Quote:

Originally Posted by Niru (Post 442604)
BTW
Your work on "Numerical modeling of pool spreading,
heat transfer and evaporation in
liquefied natural gas (LNG)" was good. I am assuming that you wrote this thesis.

Yes, you are correct - this is my master's thesis. And thank you! :) How did you come by it anyway? Boiling of LNG (or mixtures in general) is a relatively small research field.

oystein_myrmo August 4, 2013 08:02

Quote:

Originally Posted by Lieven (Post 442609)
Hi all,

Although it seems like a very simple problem to set the boundary conditions, it is actually quite tricky. Have a look at the following papers for more information:

* Richards, P., & Hoxey, R. (1993). Appropriate boundary conditions for computational wind engineering models using the k-ϵ turbulence model. Journal of Wind Engineering and Industrial Aerodynamics, 47, 145153.
* Blocken, B., Stathopoulos, T., & Carmeliet, J. (2007). CFD simulation of the atmospheric boundary layer: wall function problems. Atmospheric Environment, 41(2), 238252. doi:10.1016/j.atmosenv.2006.08.019
* Sumner, J., & Masson, C. (2011). k- epsilon simulations of the neutral atmospheric boundary layer: analysis and correction of discretization errors on practical grids. International Journal for Numerical Methods in Fluids. doi:10.1002/fld

It is for example very tempting to set the slip condition at the top of the domain but this will introduce a modeling error which, depending on the extent of the domain, can become non-negligible...

Cheers,

Lieven

Thank you, Lieven - I will look into these papers. Do you by chance know if the same problems apply to other turbulence models as well? Will it be different when using for example Reynold's Stress Model?

Niru August 4, 2013 08:25

thesis
 
I am working on LNG pool spreading and evaporation. I am developing my own model for it . Have you graduated? Can you share your experience on working with that topic?

oystein_myrmo August 4, 2013 12:35

thesis
 
Cool! Check your personal inbox, so we can continue on topic here ;)

Lieven August 4, 2013 18:24

I didn't test other models on the problem (simply because the k-epsilon model is the most frequently used model for this situation). But I'm pretty sure that this issue will be present in the other models too but maybe not to the same extent.

Cheers,

L

Eloise August 6, 2013 05:04

Quote:

Originally Posted by oystein_myrmo (Post 443719)
Thank you, Lieven - I will look into these papers. Do you by chance know if the same problems apply to other turbulence models as well? Will it be different when using for example Reynold's Stress Model?

Hello ystein,

For different turbulence models, please check as well this reference:
Richards, P. J., and S. E. Norris. "Appropriate boundary conditions for computational wind engineering models revisited." Journal of Wind Engineering and Industrial Aerodynamics 99.4 (2011): 257-266.


Best regards,
Elose

oystein_myrmo August 13, 2013 05:21

Thank you for the reference, Eloise.

I have digged into the atmBoundaryLayerInletVelocity and atmBoundaryLayerInletEpsilon boundary conditions, and I find it a bit strange that the roughness length (z0_), the minimum coordinate in z-direction (zGround_) and friction velocity (Ustar_) are all defined as scalarFields of the same size as the patch where the BC is applied. Shouldn't all of these parameters be constants (i.e. scalar) in the wind profile?

I see in the implementation of atmBoundaryLayerInletVelocityFvPatchVectorField that Ustar_[i] is calculated depending on z0[i] like this:

Code:

forAll (Ustar_, i)
{
    Ustar_[i] = kappa_*Uref_/(log((Href_  + z0_[i])/max(z0_[i] , 0.001)));
}

and the calculation of the velocity itself (Un) depends on all of Ustar_[i], zGround_[i] and z0_[i] like this:

Code:

forAll(coord, i)
{
    if ((coord[i] - zGround_[i]) < Href_)
    {
        Un[i] =
            (Ustar_[i]/kappa_)
            * log((coord[i] - zGround_[i] + z0_[i])/max(z0_[i], 0.001));
    }
    else
    {
        Un[i] = Uref_;
    }
}

What's the reason the BC is implemented in this way? Also, why is the boundary layer truncated at Uref_ and forcing it to remain constant from thereon? Since this BC is of type fixedValueFvPatchVectorField the calculation of the values is only done once (?) and thus the log calculations are also done only once.

Can anyone enlighten me on these issues?

Eloise August 14, 2013 07:23

Hello ystein,

A simple way to test your BCs is to run an "empty fetch case", i.e. an empty 2D domain on which you use your set of BCs. By comparing your inlet and outlet profiles of U k and epsilon, you will be able to see if your set of BCs are consistent.

I haven't try to use the atmBoundaryLayer BCs from OpenFOAM, but I'd not be surprised if it did not maintain the profiles through the domain. Instead, I'd recommend you to implement the recommendations suggested in the above mentioned papers.

Regards,
Elose

kingjewel1 March 17, 2014 14:09

Did anybody determine whether they were happy with the way the ABL is currently modelled by atmBoundaryLayerInletVelocity?

To be honest i'm a bit puzzled as to how to implement a turublent gradient at the ceiling of the domain as suggested in "Appropriate boundary conditions for computational wind engineering models revisited". Any thoughts here?

allett02015 June 23, 2015 05:49

2 Attachment(s)
Hello!

Did anyone find a solution to the above Problems? I have the same problem. I applied nutkAtmRoughWallFunction and epsilon wall functions at the wall.

In order to test if the solution optained with openfoam is consistent with the theory I used a 2D channel an applied a cyclic bounday condition at inlet and outlet. At the top of the domain a used a constant velocity.

It is some kind of couette flow.

Theoretically the converged velocity solution should be logarithmic at the wall U = U*/kappa ln ( ( z + z0)/z0)). Unfortunately I did not get the theretical profile.

Find attached the plot of the velocity

allett02015 June 30, 2015 05:27

Hello! I've tried to implement the discretisation of the Production therm suggesteb by

Richards, P. J., and S. E. Norris. "Appropriate boundary conditions for computational wind engineering models revisited." Journal of Wind Engineering and Industrial Aerodynamics 99.4 (2011): 257-266.

In openfoam it looks like :

volVectorField snGradU("snGradU",fvc::average(fvc::snGrad(U_) ) );
volScalarField G(GName(), nut_*magSqr( snGradU ) );

So I compute first the face area avereg of the gradient and then squared it to get the Production term G.

But still I got a turbulent lengthcale which is increasing with hight with a lower inclination compared to kappa*z. Did anyone try this solution?

wc34071209 August 25, 2016 06:57

Is there any progress regarding this problem?

allett02015 August 26, 2016 04:00

unfortunately I was not able to solve the problem. but it is definitely a numerical issue. If you use an equidistant mesh an use a very fine resolution the spike of k at the bottom vanishes.

Another guess of me was that the reason is the first order approximation of the velocity gradient at the wall in the calculating the turbulent production.

but I hadn't the time to test if this assumption is right.


All times are GMT -4. The time now is 21:34.