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

Boundary Conditions for v2f turbulent model

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

Like Tree22Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   April 2, 2013, 12:05
Question Boundary Conditions for v2f turbulent model
  #1
New Member
 
Blaž Mikuž
Join Date: Sep 2011
Location: Ljubljana
Posts: 29
Rep Power: 6
bmikuz is on a distinguished road
Hello,

I noticed that the new version of OF 2.2.0 contains implemented v2f turbulent model. Now, I'd like to use that model for flow in a channel or for flow through a tube. The problem is that there is no prepared case using v2f turbulent model in $FOAM_TUTORIALS directory, where one can see how to set the boundary conditions (BCs).

I realized that you need 7 fields in 0 directory: U, p, nut, k, epsilon, f and v2.
Firstly, what are correct dimensions for f and v2? Is dimension (1/s) for f and (m^2/s^2) for v2 correct?
Secondly, what should be proper BC for f and v2 on the outlet? I followed the instructions for BC written in v2f.H file, but found them little incomplete...

Thanks in advance for your help or any comment.
Blaz
bmikuz is offline   Reply With Quote

Old   April 2, 2013, 12:59
Default
  #2
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 381
Rep Power: 12
cnsidero is on a distinguished road
bmikuz,

The v^2-f model was one of the turbulence models I investigated for my doctoral research. From the literature the following is what I learned to use for v^2 and f boundary conditions.

Inlet:

v^2 = \frac{2}{3}\,k_{inlet}
\frac{\partial f}{\partial n} = 0

Outlet:
zero gradient for both

Walls:

v^2 = 0.0

f = \frac{20\,\nu^2\,v^2}{\varepsilon_{inlet}\,y^4}

If you want the justification and full discussion, I'll refer you to the original v^2-f paper by Paul Durbin and a PhD thesis by Andreas Sveningsson:

Durbin, P.A., 1991 “Near-Wall Turbulence Closure Modeling Without ‘Damping Functions”’ Theoretical and Computational Fluid Dynamics Vol. 3, pp. 1-13

Sveningsson, A. 2003 “Analysis of the Performance of Different v^2-f Turbulence Models in a Stator Vane Passage Flow”, Ph.D Thesis, Chalmers University of Technology ISSN 1101-9972
http://publications.lib.chalmers.se/...e-passage-flow

In particular, I found Sveningsson's thesis very helpful.

And by the way, the v^2-f requires full resolution of the boundary layer, i.e. y+ <= 1.

Hope that helps, Chris

Quote:
Originally Posted by bmikuz View Post
Hello,

I noticed that the new version of OF 2.2.0 contains implemented v2f turbulent model. Now, I'd like to use that model for flow in a channel or for flow through a tube. The problem is that there is no prepared case using v2f turbulent model in $FOAM_TUTORIALS directory, where one can see how to set the boundary conditions (BCs).

I realized that you need 7 fields in 0 directory: U, p, nut, k, epsilon, f and v2.
Firstly, what are correct dimensions for f and v2? Is dimension (1/s) for f and (m^2/s^2) for v2 correct?
Secondly, what should be proper BC for f and v2 on the outlet? I followed the instructions for BC written in v2f.H file, but found them little incomplete...

Thanks in advance for your help or any comment.
Blaz
anothr_acc, fumiya, bmikuz and 3 others like this.
cnsidero is offline   Reply With Quote

Old   April 2, 2013, 16:18
Default
  #3
New Member
 
bscphil's Avatar
 
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5
bscphil is on a distinguished road
@bmikuz: I have do some simulations with the new v2f turbulence model (the incompressible version) in OpenFOAM 2.2.0 and give you my boundary conditions. I think it can help you

U:
Code:
dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (1 0 0);

boundaryField
{
    inlet
    {
      
        type            fixedValue;
        value           nonuniform List<vector> 
64
(
(0.111708 6.41525e-06 0)
(0.322171 -1.26309e-05 0)
(0.488089 5.5452e-06 0)
(0.601945 -1.16204e-07 0)
(0.681378 1.39714e-06 0)
(0.74007 3.13196e-06 0)
(0.785756 4.7772e-06 0)
(0.822917 6.06065e-06 0)
(0.854232 6.85654e-06 0)
(0.881348 7.05289e-06 0)
(0.905324 6.60611e-06 0)
(0.926875 5.52305e-06 0)
(0.946502 3.84961e-06 0)
(0.964567 1.65758e-06 0)
(0.98134 -9.65316e-07 0)
(0.997026 -3.92283e-06 0)
(1.01178 -7.11429e-06 0)
(1.02574 -1.04334e-05 0)
(1.03898 -1.37726e-05 0)
(1.0516 -1.70166e-05 0)
(1.0636 -2.00434e-05 0)
(1.075 -2.27193e-05 0)
(1.08579 -2.48985e-05 0)
(1.0959 -2.64265e-05 0)
(1.10529 -2.71472e-05 0)
(1.11386 -2.69128e-05 0)
(1.12153 -2.55954e-05 0)
(1.12819 -2.3057e-05 0)
(1.13373 -1.94304e-05 0)
(1.13809 -1.47821e-05 0)
(1.14115 -9.3311e-06 0)
(1.14277 -3.1689e-06 0)
(1.14277 3.30393e-06 0)
(1.14115 9.46547e-06 0)
(1.13809 1.49146e-05 0)
(1.13373 1.9562e-05 0)
(1.12819 2.31885e-05 0)
(1.12153 2.57287e-05 0)
(1.11386 2.70509e-05 0)
(1.10529 2.72948e-05 0)
(1.0959 2.65897e-05 0)
(1.08579 2.50852e-05 0)
(1.075 2.29391e-05 0)
(1.0636 2.03078e-05 0)
(1.0516 1.73391e-05 0)
(1.03899 1.41684e-05 0)
(1.02574 1.09186e-05 0)
(1.01178 7.70432e-06 0)
(0.997028 4.63039e-06 0)
(0.981344 1.79609e-06 0)
(0.964572 -7.09707e-07 0)
(0.946509 -2.80824e-06 0)
(0.926884 -4.43494e-06 0)
(0.905335 -5.54543e-06 0)
(0.88136 -6.12197e-06 0)
(0.854244 -6.18138e-06 0)
(0.822926 -5.77808e-06 0)
(0.785759 -5.0163e-06 0)
(0.740064 -4.00941e-06 0)
(0.68136 -2.93789e-06 0)
(0.601916 -1.92725e-06 0)
(0.488061 -7.47706e-06 0)
(0.322159 1.1563e-05 0)
(0.111704 -6.52362e-06 0)
)
;
    }
    outlet
    {
        type            zeroGradient;
    }
    walls
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    frontAndBack
    {
        type            empty;
    }
}


p:
Code:
dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    walls
    {
        type            zeroGradient;
    }
    frontAndBack
    {
        type            empty;
    }
}


epsilon:
Code:
dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 3.825E-5;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 3.825E-5;
    }
    outlet
    {
        type            zeroGradient;
    }
    walls
    {
        type            zeroGradient;
    }
    frontAndBack
    {
        type            empty;
    }
}


k:
Code:
dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 3.75E-3;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 3.75E-3;
    }
    outlet
    {
        type            zeroGradient;
    }
    walls
    {
        type            fixedValue;
        value           uniform 1.0E-15;
    }
    frontAndBack
    {
        type            empty;
    }
}


nut:
Code:
dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            calculated;
        value           uniform 0;
    }
    outlet
    {
        type            calculated;
        value           uniform 0;
    }
    walls
        {
//        type            calculated;
//        value           uniform 0;

      type            zeroGradient;

//      type            nutLowReWallFunction;
//      value           uniform 0;
    }

    frontAndBack
    {
        type            empty;
    }
}


v2: v2(inlet) = 2/3*k(inlet)
Code:
dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 2.5e-3;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value           uniform 2.5e-3;
    }
    outlet
    {
        type            zeroGradient;
    }
    walls
    {
        type            fixedValue;
        value           uniform 1e-10;
    }
    frontAndBack
    {
        type            empty;
    }
}


f:
Code:
dimensions      [0 0 -1 0 0 0 0];

internalField   uniform 1e-10;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
    }
    walls
    {
        type            fixedValue;
        value           uniform 1e-10;
    }
    frontAndBack   
    {
        type            empty;
    }
}


I hope this helps you. Other assuptions for my case are:
  1. the case is a "low-Re" turbulence modeling case without any wallFunctions
  2. the walls have patch-type "wall", to use the "nutLowReWallFunction" for calculating the yPlus values
  3. the yPlus values are between 0.3 and 7 (calculated with the "nutLowReWallFunction" --> yPlus should be approx 1 !! but results are ok...
  4. for the velocity inlet condition i use a fully developed velocity profile. This is calculated befor e.g. with the "LaunderSharmaKE" turbulence model.
  5. i have compared my results with experimental results from the ERCOFTAC Case 8.2 (Flow through an Asymetric diffuser) http://www.ercoftac.org/fileadmin/us...8.2/index.html
  6. the results are good for the mean-velocity and the distributions of skin friction coefficients are plausible (i see transition and re-attechment points)
@cnsidero: thanks for the references
anothr_acc, fumiya, bmikuz and 3 others like this.
bscphil is offline   Reply With Quote

Old   April 3, 2013, 10:42
Default
  #4
New Member
 
Blaž Mikuž
Join Date: Sep 2011
Location: Ljubljana
Posts: 29
Rep Power: 6
bmikuz is on a distinguished road
Thanks a lot @cnsidero and @bscphil. You were of great help!

I used @bscphil's BCs and a "tutorial" simulation works now. Since my real case is quite big and contains a lot of vanes inside a tube, I cannot afford very dense mesh in the boundary layer. So my next step is using wall functions, which are also implemented in that v2f turbulent model...
bmikuz is offline   Reply With Quote

Old   April 3, 2013, 10:50
Default
  #5
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 381
Rep Power: 12
cnsidero is on a distinguished road
Good to hear.

Seems kind of dubious to me to use wall functions with the v2-f. The whole purpose of adding the v2 and f equations to the k-e model was to provide better scaling of the turbulent kinetic energy near the wall. The Durbin paper I reference discusses this at length. My point is, if you're going to use a wall-function with the v2-f, which will effectively override the benefit of the v2-f model, it's seems pointless to use it.

Just my $0.02.

Quote:
Originally Posted by bmikuz View Post
Thanks a lot @cnsidero and @bscphil. You were of great help!

I used @bscphil's BCs and a "tutorial" simulation works now. Since my real case is quite big and contains a lot of vanes inside a tube, I cannot afford very dense mesh in the boundary layer. So my next step is using wall functions, which are also implemented in that v2f turbulent model...
cnsidero is offline   Reply With Quote

Old   April 3, 2013, 11:29
Default
  #6
New Member
 
Blaž Mikuž
Join Date: Sep 2011
Location: Ljubljana
Posts: 29
Rep Power: 6
bmikuz is on a distinguished road
Ok, good to know that. I don't know much about the v2f turbulent model yet, but I checked the Description in the v2f.H file (attached to the post) and there are somehow recommended wall boundary conditions as follows:

k=kLowReWallFunction
epsilon=epsilonLowReWallFunction
v2=v2WallFunction
f=fWallFunction

There must be a good reason for implementing these wall functions in v2f model or isn't it?
Attached Files
File Type: h v2f.H (7.6 KB, 73 views)
bmikuz is offline   Reply With Quote

Old   April 3, 2013, 11:53
Default
  #7
Senior Member
 
Chris Sideroff
Join Date: Mar 2009
Location: Ottawa, ON, CAN
Posts: 381
Rep Power: 12
cnsidero is on a distinguished road
Quote:
Originally Posted by bmikuz View Post
There must be a good reason for implementing these wall functions in v2f model or isn't it?
My guess is to make it more robust for practical applications. Specifically I mean for complex applications it may be difficult to generate mesh that meets y+ requirement everywhere.

But in general, the formulation of the v2-f was develop to handle resolved flows better than other 2 equation formulations of the k-e. I did notice in the v2f.H header they reference some newer papers, which I haven't read, but it's possible that they discuss near wall handling of v2 and f for y+ > 1.

So while it can handle y+ > 1, my understanding of its benefit is that you should try to keep y+ <= 1. Of course, some validation against some know applications that demonstrate the v2-f benefits might be a good exercise.

FYI, the near wall v2 and f behaviors are defined in v2WallFunctionFvPatchScalarField.C and fWallFunctionFvPatchScalarField.C where it checks for the yPlusLam value (edge of viscous sub-layer) and switches accordingly.
alquimista, fumiya and bmikuz like this.

Last edited by cnsidero; April 4, 2013 at 08:59.
cnsidero is offline   Reply With Quote

Old   April 3, 2013, 18:52
Default
  #8
New Member
 
bscphil's Avatar
 
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5
bscphil is on a distinguished road
Quote:
Originally Posted by cnsidero View Post
But in general, the formulation of the v2-f was develop to handle resolved flows better than other 2 equation formulations of the k-e. I did notice in the v2f.H header they reference some newer papers, which I haven't read, but it's possible that they discuss near wall handling of v2 and f for y+ > 1.
Ok, my understanding is the same, the v2f turbulence model is a socalled "low"-Re turbulence model (also for high Re-Numbers in the core flow) with no use of any wall functions, because of a resolved boundary layer. The differences between "high"- and "low"-Re models is in the attached figure "itw_vs_wtf.jpg".

For me it make no sense to use wall functions in the v2f-model (don't know what the OpenFOAM developer want to do with these ?? ). I have read all newer and older papers about the v2f model and i dosn't find any near wall handling of v2 and f for y approx 30 like in an "high"-Re model.

I read the v2f.H-file too and spend some time to simulate my diffuser testcase with the use of all wall functions ...

the results with the use of wall functions are very bad:
  1. f and v2 becomes infinity field values
  2. the residuals swing a lot and there was no convergence
  3. the velocity and pressure field looks normal, but i don't have the near wall seperation bubble like in my simulation without wall functions
  4. the mean velocity and skin friction distributions in comparison with the experimental data are very bad (see atteched plots "Ux_..." and "cf_..." --> the red lines are without wall functions and the green lines are with wall functions)
I have two possibilites for you:
  1. refine your mesh at the no-slip walls to have y+<1 (or firstly y+<5-7)...use some boundary layers at your walls (5-10 layers maybe)
  2. use another turbulence model, for example any of the "high"-Re turbulence models and then u can use your wall functions
@all: when i don't right with my assumptions then let me know, please !!!
Attached Images
File Type: jpg itw_vs_wf.jpg (29.5 KB, 143 views)
File Type: jpg cf_asymetric_diffuser.jpg (38.6 KB, 149 views)
File Type: jpg Ux_asymetric_diffuser.jpg (18.2 KB, 106 views)
fumiya, bmikuz and mgg like this.
bscphil is offline   Reply With Quote

Old   April 4, 2013, 05:34
Default
  #9
New Member
 
Blaž Mikuž
Join Date: Sep 2011
Location: Ljubljana
Posts: 29
Rep Power: 6
bmikuz is on a distinguished road
Thanks for instructions to both of you. Since I already did a simulation with k-omega SST turbulence model (with wall functions), I'll have to follow your first suggestion @bscphil and add more layers at the walls. I hope that the mesh will not become significantly bigger than it is now (~40 millions cells).

About the @bscphil's testing of wallfunctions on diffusor: were the meshes of the same size in both cases (with and without wallfunctions)?
bmikuz is offline   Reply With Quote

Old   April 4, 2013, 19:30
Default
  #10
New Member
 
bscphil's Avatar
 
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5
bscphil is on a distinguished road
Quote:
Originally Posted by bmikuz View Post
About the @bscphil's testing of wallfunctions on diffusor: were the meshes of the same size in both cases (with and without wallfunctions)?
I have good news the velocity field with the use of wall functions have good comparison to the experimental data

To your question, no the meshes don't have the same size, because of wall functions i use a coarse mesh at the walls. I think about my case and i find my mistake, i used for the simulation with wall functions the mapped field of my first post for the velocity, this field was calculated with the "low-Re" LaunderSharmaKE model and represent a fully developed channel flow with near wall resolution --> i cancel this and use for velocity at the inlet:
Code:
inlet
    {     
        type            fixedValue;
        value           uniform (1 0 0);
    }
Now i get better results with the use of wall functions, but i have some "building sites":
  1. my residuals for v2, f and p are not so good, they swing a lot and are high
  2. the fields for v2 and f have some differences to the same fields with the calculation without wall functions (see atteched pictures)
  3. the skin friction distributions are ok for the lower wall (the seperation point is exactly the point of experiment, a wonder? ) and not so good for the upper wall in comparison with the experiments
  4. the seperation bubble is at the right position
  5. i don't have plot the pressure coefficients, maybe i can do this?
You said that you have a channel or tube flow with some vanes inside...i have some questions to you:
  1. have you a full 3D tube? when yes, why don't you use a little part like a 10-45 degree piece of the tube for your calculation (with cyclic/periodic boundary conditions at the cutting planes)...then you can have a finer mesh
  2. What's the Re-number for your case?
  3. Which solver you use? --> just describe us your case, please
I hope i can help you for the first time?

(--> the red lines are without wall functions and the green lines are with wall functions !!)
Attached Images
File Type: png cf_asymetric_diffuser.png (57.1 KB, 100 views)
File Type: jpg diffuser_v2f_withoutWF_f.jpg (25.7 KB, 86 views)
File Type: jpg diffuser_v2f_withoutWF_streamlines.jpg (40.5 KB, 84 views)
File Type: jpg diffuser_v2f_withoutWF_v2.jpg (25.8 KB, 78 views)
Attached Files
File Type: pdf Ux_asymetric_diffuser.pdf (29.7 KB, 44 views)

Last edited by bscphil; April 5, 2013 at 04:27.
bscphil is offline   Reply With Quote

Old   April 4, 2013, 19:33
Default
  #11
New Member
 
bscphil's Avatar
 
Phillip
Join Date: Mar 2012
Location: Germany
Posts: 27
Rep Power: 5
bscphil is on a distinguished road
ok the limit for upload stopped me, here is the rest....
Attached Images
File Type: jpg diffuser_v2f_withWF_f.jpg (25.1 KB, 56 views)
File Type: jpg diffuser_v2f_withWF_streamlines.jpg (37.5 KB, 56 views)
File Type: jpg diffuser_v2f_withWF_v2.jpg (24.9 KB, 50 views)

Last edited by bscphil; April 5, 2013 at 04:27.
bscphil is offline   Reply With Quote

Old   April 8, 2013, 04:48
Default
  #12
New Member
 
Blaž Mikuž
Join Date: Sep 2011
Location: Ljubljana
Posts: 29
Rep Power: 6
bmikuz is on a distinguished road
First, my apology for late reply.
Thanks for sharing your results, which are more promising for me.

My "tutorial" case was flow in a circular tube just to initiate/try v2f model. Now I want to use v2f for my "real" case, which is flow through fuel bundle of nuclear reactor. To be more specific, in my case fuel bundle is an array of 5×5 fuel rods which are held together with spacer grid (in the middle of sketch geo.jpg). At the outlet of spacer grid there are mixing vanes (spacer1.jpg), which serve for increasing the turbulence of the flow... So, the coolant (water) is flowing in a square channel along the rods. Reynolds number is around 50000, I want to run transient simulation with pisoFoam. Benchmark will be done with experimental measurements of velocity fields behind mixing vanes, so I'm not interested in skin frictions...

Since I'm interested in velocity fields, the simulation with wall functions may be good enough? I'll probably prepare both simulations (with & without wall functions) but it will take some more time.
Attached Images
File Type: jpg geo.jpg (35.8 KB, 49 views)
File Type: jpg spacer1.jpg (48.2 KB, 49 views)
bmikuz is offline   Reply With Quote

Old   March 24, 2014, 12:53
Default
  #13
New Member
 
Join Date: Mar 2012
Posts: 13
Rep Power: 5
Maff is on a distinguished road
Since I've been working with the v2f model for a while, I wanted to share with you some thoughts about the wall conditions.
For the v2f model implemented in openfoam, the boundary conditions at the wall for low-re cases are:
k=1e-10
v2=1e-10
f=1e-10 (because of the code-friendly modification by Lien)
nut=nutLowReWallFunction(i.e. =0)
epsilon is not zero nor zeroGradient.
epsilon = 2*nu*k1/y1^2, where k1 and y1 are the cell-center values at the wall.
The wall function implemented in openfoam is supposed to take care of it (epsilonLowReWallFunction).
But I had some problems using it, it makes the simulation diverge.
I had a look at the code:
Code:
if (yPlus > yPlusLam_)
        {
            epsilon[cellI] = w*Cmu75*pow(k[cellI], 1.5)/(kappa_*y[faceI]);
        }
        else
        {
            epsilon[cellI] = w*2.0*k[cellI]*nuw[faceI]/sqr(y[faceI]);
        }

        G[cellI] =
            w
           *(nutw[faceI] + nuw[faceI])
           *magGradUw[faceI]
           *Cmu25*sqrt(k[cellI])
           /(kappa_*y[faceI]);
I think it should be:
Code:
if (yPlus > yPlusLam_)
        {
            epsilon[cellI] = w*Cmu75*pow(k[cellI], 1.5)/(kappa_*y[faceI]);
			
            G[cellI] =
                w
               *(nutw[faceI] + nuw[faceI])
               *magGradUw[faceI]
               *Cmu25*sqrt(k[cellI])
               /(kappa_*y[faceI]);
        }
        else
        {
            epsilon[cellI] = w*2.0*k[cellI]*nuw[faceI]/sqr(y[faceI]);
        }
With this modification, the wall function is working for me.
If you want it, I'm attaching it to this post.
it is called myEpsilonLowReWallFunction.
just compile it and then add this to controldict:
Code:
libs ( "myEpsilonLowReWallFunction.so" );
If you want to avoid this, you should get the same results with groovyBC:
Code:
        type            groovyBC;
        valueExpression "2*nu*internalField(k)/sqr(mag(delta()))";
        value           uniform 1e-10;
Attached Files
File Type: zip myEpsilonLowReWallFunction.zip (8.4 KB, 51 views)
anothr_acc, er_trebbia and JanBVB like this.
Maff is offline   Reply With Quote

Old   November 20, 2015, 06:22
Default
  #14
Member
 
SM
Join Date: Dec 2010
Posts: 82
Rep Power: 7
canopus is on a distinguished road
Hi, I tried to use the v2f model in OF and for that I ran boundaryFoam and compared to Channel395 DNS.
For High Reynolds Number (HRN) model (y+ > 30) I got quite good results with OpenFOAM recommended settings i.e. as attached

Wall settings
Code:
k       = kLowReWallFunction                                        
 epsilon = epsilonLowReWallFunction 
v2      = v2WallFunction                                         
f       = fWallFunction
nut     = nutUSpaldingWallFunction;
But on trying to use in Low Reynolds Number (LRN) version (y+ <1 ) it gives weird result.

After googling and trying all possible combinations I got the best (yet not good) from following combination

Wall settings
Code:
k       = kLowReWallFunction                                         
epsilon = fixedValue 1e-10 
v2      = v2WallFunction                                         
f       = fWallFunction
nut     = zeroGradient
My observations are that most important factors are
setting nut = zeroGradient and epsilon = fixedValue (1e-10) at walls.

If you use any other as nutLowReWallFunction or epsilonLowReWallFunction results are way off.
For k,v2,f you can also use fixedValue (1e-10) and results are same.

Anyone else has same observations?
Or wants to test can ask for case files.
Attached Images
File Type: png recomendedHRNv2f.png (21.3 KB, 26 views)
File Type: png recomendedLRNv2f.png (29.6 KB, 23 views)
File Type: png zerogradNutLRNv2f.png (25.9 KB, 24 views)
canopus is offline   Reply With Quote

Old   November 21, 2015, 07:24
Default
  #15
New Member
 
Join Date: Mar 2012
Posts: 13
Rep Power: 5
Maff is on a distinguished road
In my experience, results like that in your second figure are usually caused by an early divergence of the turbulence variables (you might see huge values for k or v2 near the walls).
It may still give you a result, but it will not be a physical one.
I wouldn't play too much with the boundary conditions, there are physical reasons to use nutLowReWallFunction and epsilonLowReWallFunction.
The initialization is usually the key: try and use a low-re k-epsilon model first, like LaunderSharmaKE (remember to use epsilon=0 at the wall with that model) or AbeKondohNaganoKE (Abe-Kondoh-Nagano low-Re k-epsilon model).
Maff is offline   Reply With Quote

Old   November 23, 2015, 09:34
Default v2 wall boundary condition
  #16
New Member
 
Join Date: Jun 2014
Posts: 2
Rep Power: 0
Kire is on a distinguished road
Hi

I have a question about the v2 boundary condition in v2WallFunction.

Code:
   // Set v2 wall values
    forAll(v2, faceI)
    {
        label faceCellI = patch().faceCells()[faceI];

        scalar uTau = Cmu25*sqrt(k[faceCellI]);

        scalar yPlus = uTau*y[faceI]/nuw[faceI];

        if (yPlus > yPlusLam_)
        {
            scalar Cv2 = 0.193;
            scalar Bv2 = -0.94;
            v2[faceI] = Cv2/kappa_*log(yPlus) + Bv2;
        }
        else
        {
            scalar Cv2 = 0.193;
            v2[faceI] = Cv2*pow4(yPlus);
        }

        v2[faceI] *= sqr(uTau);
    }
From the references Lien and Kalitzin (2001), it seems v2 approaches O(y^4) as y ---> 0, but how is v2[faceI] = Cv2*pow4(yPlus) derived? Where does this Cv = 0.193 come from?

Also, due to my poor c++ skills, I wonder why v2 gets multiplied by sqr(uTau) and assigned the value after the if loop? What is the purpose of that?

Thanks.
Kire is offline   Reply With Quote

Old   November 23, 2015, 10:36
Default
  #17
New Member
 
Join Date: Mar 2012
Posts: 13
Rep Power: 5
Maff is on a distinguished road
you will find everything in this paper:
Kalitzin et al. 2004. Near-wall behavior of RANS turbulence models and implications for wall functions.
In the if loop v2 is actually v2Plus, that's why you multiply it by sqr(uTau).
Kire likes this.
Maff is offline   Reply With Quote

Old   November 24, 2015, 14:39
Default
  #18
New Member
 
Karl Lindqvist
Join Date: Jul 2012
Location: Trondheim, Norway
Posts: 11
Rep Power: 5
karlli is on a distinguished road
Dear all,
I'd just like to add my small piece of insight in this issue, after also struggling to understand the OF wall functions.

It turns out that there was a bug in the epsilonLowReWallFunction up to and including version 2.4.x, causing erratic behavior of this wall function. Just as canopus, I got some very wierd profiles for velocity and turbulent kinetic energy for a channel flow test case despite good initialization.

Using the wall function implementation in v.3.0.0 gives much better results. The alternative approach (setting v2,f,k to machine zero, epsilon to zeroGradient as explained here) also give reasonable results (green curve).

So to conclude, it seems like the new wall functions reduce to the low-Re approach (more or less) for small y+ values.
Attached Images
File Type: png a.png (42.2 KB, 24 views)
File Type: png b.png (39.0 KB, 26 views)
karlli is offline   Reply With Quote

Old   November 25, 2015, 04:01
Default
  #19
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 1,010
Rep Power: 18
akidess will become famous soon enough
For sake of completeness, I'm guessing you are referring to bug ID 0001852, resolved by 9bf69ecd0bb19deb1bdfa5d2bb7034b6559242ea:

http://www.openfoam.org/mantisbt/view.php?id=1852

Quote:
Originally Posted by karlli View Post
Dear all,
I'd just like to add my small piece of insight in this issue, after also struggling to understand the OF wall functions.

It turns out that there was a bug in the epsilonLowReWallFunction up to and including version 2.4.x, causing erratic behavior of this wall function. Just as canopus, I got some very wierd profiles for velocity and turbulent kinetic energy for a channel flow test case despite good initialization.

Using the wall function implementation in v.3.0.0 gives much better results. The alternative approach (setting v2,f,k to machine zero, epsilon to zeroGradient as explained here) also give reasonable results (green curve).

So to conclude, it seems like the new wall functions reduce to the low-Re approach (more or less) for small y+ values.
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Join the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oHPxcPqde7HtA2
akidess is offline   Reply With Quote

Old   January 16, 2016, 17:36
Default
  #20
Member
 
SM
Join Date: Dec 2010
Posts: 82
Rep Power: 7
canopus is on a distinguished road
"epsilon to zeroGradient" for Low Re Turbulence models?

Are you sure ?
In the tutorial folder

Quote:
tutorials/incompressible/boundaryFoam/boundaryLaunderSharma/0
for walls epsilon is set to

Code:
lowerWall
    {
        type            fixedValue;
        value           uniform 1e-08;
    }
canopus is offline   Reply With Quote

Reply

Tags
boundary conditions, v2f, wall functions

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 41 February 2, 2016 07:48
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 17:44
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
Copying boundary conditions from model to model Lior FLUENT 3 September 23, 2004 16:10


All times are GMT -4. The time now is 08:53.