Friction forces in Interfoam
 

Hi everyone

I need to modelise numerically and physically a spillway.

I made some measures in the physical reduced model and now I would like

to adjust my numerical results in interfoam.

Do you know how is modelised the frictions forces in interfoam?
What are the parameters I could change to adjust my results?

Thank you

Hi Trapan,

The friction forces are calculated in the boundary conditions for nut. If you look in the tutorials for interfoam (ras), you will notice that in the weirOverflow and the waterChannel tutorials the nutkWallFunction condition is used. This condition refers to a smooth wall. On the other hand the DTCHull tutorial uses the nutkRoughWallFunction condition which is a rough wall. The roughness is defined by the ks parameter which is the same roughness that is used in the Moody diagram.

Best regards,
Paulo

Thank you very much for your help

Turbulence model
 

I have a new question about the turbulence i InterFoam.

I am in internship and i have to modelize the spillway numerically and physically.

During the physical modelling, I saw a "karman vortex" around the upstream wall of the spillway.

However, in the numerical simulation I don't see this phenomenon when I visualized my results in Paraview.

I am using Interfoam and the k-omega-SST RAS turbulence model.

Do you know how can I represent the karman vortex ?

Thank you

Hi Trapan,

Looking at the photo and the visualization it seems that there are some differences in the upstream geometry. It seems that, in the simulation, the fluid goes directly to the spillway and in the physical model the fluid arrives sideways making a curve. This may be the cause of the vortex you are observing. Try to change the simulation geometry to reproduce more precisely the model. It its possible that you get the same vortex.

Best regards,
Paulo

Hi Paulo,

I have another question and I hope you could help me.
I am trying to match my numerical model with the physical one.

So, first of all, I made a sensibility analysis and I found that the nut parameter is the parameter which influenced the most my results for my water level. ( It's normal because you told me that the friction forces are calculated in the boundary conditions for nut).

So now I have tried some simulations and for the upstream part the water level is good ( compared to result in the physical model) but for the downstream part I still have some différences (about 20-30cm) . Even if I change the parameter nut, the value doesn't change a lot.


You told me that the roughness is defined by the ks parameter. Do you know where I can change the value of ks ?

Thank's a lot and have a good day

For the moment I used nutkWallFunction because in reality my wall has a strickler's value of 70.
But what is the roughness coefficeint used in OpenFoam for the function nutkWallFunction?
What is represented when I change the value of nut with a nutkWallFunction?

Maybe I need to use the nutroughWallFunction.

Hi Trapan,

The nutkWallFunction is for a smooth wall, it may be applied when the roughness is very small. For a rough wall you should use nutroughWallFunction. An example of the use of this condition appears in the DTCHull tutorial, in the hull surface you have:

hull
{
type nutkRoughWallFunction;
Ks uniform 100e-6;
Cs uniform 0.5;
value $internalField;
}

The "Cs" value is always 0.5, "Ks" is the roughness in meters and "value" is an initial estimate for nut.

The relation between the Strikler coefficient and Ks depends on the Reynolds number. Here in Brasil there is a very popular Hydraulics book that gives the following relation between the roughness and the Strickler coefficient Ks=(25.6/kstr)^6 where kstr is the Strikler coeficcient. This is an approximate formula valid for very high Reynolds numbers.

Best Regards,
Paulo

Hi Paulo,

Thank you again for your help.

SO I try to match my numerical model with my results of my physical model.

In the reality the Strickler value is 70. So if I used your formula
Ks=(25.6/kstr)^6 so in my case Ks= 0.00239. and Cs=0.5.

When I measured at some points the water level of my flow I have an error of 40cm with my physical model.

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -1 0 0 0 0];
internalField uniform 1e-3;
boundaryField
{
inletAir
{
type fixedValue;
value $internalField;
}

inletWater
{
type fixedValue;
value $internalField;
}
outlet
{
type zeroGradient;
}
atmosphere
{
type zeroGradient;
}
Wall
{
type nutkRoughWallFunction;
Ks 0.00239;
Cs 0.5;
value $internalField;
}

Tra
{
type nutkRoughWallFunction;
Ks 0.00239;
Cs 0.5;
value $internalField;

}


defaultFaces
{
type empty;
}
}

// ************************************************** *********************** //



Do you know which parameter I could change to increase my water lever?


Thank you again and have a good day,

Hi Trapan,

You can adjust the water level both in the inlet and outlet surfaces. This can be done in the experiment and also in the numerical model.

To adjust the water level in the inlet surface you will need to separate the inlet in two parts one is the water inlet and the other is the air inlet.

To adjust the water level in the output surface is trickier. If the bottom is horizontal, the water level will tend to the critical value
hc=((Q/b)^(2/3)) / g^(1/3)
where
hc is the critical level
Q is the flow rate
b is the channel width
g is the acceleration of gravity

If you need a level that is higher than the critical, you can put a sharp crested weir in the output region. The weir will control the water level so that you have critical level above the weir. You have to be careful to choose the position where you put the weir because it can affect the flow in a way that it becomes different than the experiment.

Best regards,
Paulo

Hi Paulo,

I'm really grateful because I succeed for match my numerical model with my physical one so thank you so much!!

Now I have, again, a new problem I can't resolve.

I tried to extend my model in making longer my chanel.

I used the same level of refinement but I don't have the same result at all. In blockMesh I created a 2 new box.
I post the result of refinement before and after extending myb channel to show you my problem.


Do you know where could be the problem?

Thank you so much

Hi!
I resolve all my problems .

I just have a question for the unit of Ks.

In the reality I have a smooth concrete and in my model I put Ks=0.1.
For this value of Ks, my numerical model is correct.

But how I could link the manning value and the Ks value?

What is the unit of Ks?

Thank you

Hi Trappan,

I've been very busy, so I couldn't answer your previous question. The manning coefficient is the inverse of the Strickler coefficient n = 1/kstr. If ks = 0.1 then using the formula from my post #8 above I get kstr = 37.6 which corresponds to n = 0.0266.

ks is given in meters so ks=0.1 corresponds to 10 cm, it is a very rough wall.

Best Regards,
Paulo

Thank you Paulo.

I understood what you explain to me. And I agree.
But my result, for a concrete channel (nearly 3m height, 3m width) are good with the value of Ks=0.1.

So I Wonder what could be the explanation.

Is it possible that my Ks is in inch and not in meters? How can I know that?

Also, I found some literature about Ks where they define it with the lengh rugosity z0.
Ks=20z0 or Ks=30z0.http://www.microwindturbine.be/Rappo...irEWEA2012.pdf

I also found that for concrete of very smooth wall (no obstacle of vegetations), z0=0.005m https://fr.wikipedia.org/wiki/Longueur_de_rugosit%C3%A9

And Ks= 20 * 0.005=0.1

I am really grateful for your help

Hi Trapan,

When you perform a CFD simulation there is always an error due to the mesh size. This error gets smaller as the size of the cells decrease. So it is important to perform some simulations with different meshes to get and ideia of the influence of the mesh in the results. In your case, it is possible that the big value of Ks is a compensation for the mesh error.

About the paper you mentioned, it is related to terrain rugosity and the wind boundary layer. It concerns a different formulation for friction forces that is used for wind simulation and it is used in OpenFOAM with other boundary conditions for nut.

Best Regards,
Paulo

Forces in interFoam laminar simulation (based on DTCHull tutorial)
 

Hello Foamers
Target of the CFD simulation - Evaluation of multi-hull ship resistance based on DTCHull. Using version 5.x. Using symmetryPlane feature.


The simulation type is laminar due to low Reynolds number (model scale simulation to compare with model scale experiment results). turbulenceProperties file is changed accordingly. In post-processing of forces, pressure and viscous forces are obtained. When obtaining the Cf (coefficient of viscous force) value, wetted surface area of half hull needs to be used (as per my understanding). However, if we use half hull wetted surface area, the viscous coefficient is not correct when compared with Blasius solution. But if we consider the full hull wetted surface area, it matches with the Blasius equation.

I am really confused with the reason for it. Therefore, now considering if the modeling of simulation (setup conditions) are correct or not.

Please help with some insights especially if you have used DTCHull tutorial.

Thanks in advance.
Sharath

Hello Paulo,


Thank you so much for your explanation of this problem! This is very useful.
But I have the question. In this case (DTCHull), the roughness (Ks) is shown for model scale (~6 meters). How I can calculate the roughness Ks for full scale ship's hull? It's will depend from the ship's length?
I have understood that the Strikler coefficient is calculate only for pipes, is it right?


Respectfully,
Serge