[mgdenno]

Hi ardjouna,

You haven't really provided enough information for me to help you. Perhaps you should have a look at this thread.

From what you said I would guess that maybe either your OF environment variables are not set properly or possibly you are using a recent version of OF but following a tutorial from an older version; recent versions use interFoam and not rasInterFoam. I think rasInterFoam may be from older versions or maybe from the extend version. I am not sure but have seen it referenced in some older posts.

If you type the following at the command:

echo $FOAM_INST_DIR

what do you see?

[ardjouna]

HI Mathiew,

Thank you for your rapid reply excuse me for not being clear
error message is:this application is not available i am working with OpenFOAM-1.5.00b-wininst it works correctly with cavity tutorial because icofoam.exe exist in Bin folder but interfoam and also rasinterfoam doesn't exist is there any way to get it for windows ?

best regards

[vonboett]

Originally Posted by MOHAMMAD67

Dear Oliver
I did all things except extending the domain. Unfortunately it didn't work and after 1.3 seconds it blows out. I don't know how deal with. I reduced the delta T to 0.00001 and turn the adjustable time step off. It is running now. I will inform you from the result.
Maybe I should make the mesh finer. Whats your opinion. Does it help me to get result.
Kind Regard

Hi Mohammad,

the issue with phase reflection at the outlet appears to several users, and type buoyantPressure; value uniform 0; usually helps. There is a funny effect: could you move your mesh to the negative coordinate quadrant (all vertices have x coordinate < 0) and check what happens at the outlet if you use type outletInlet; outletValue uniform 0; for pressure at the open boundary?

[mgdenno]

Originally Posted by ardjouna

HI Mathiew,

Thank you for your rapid reply excuse me for not being clear
error message is:this application is not available i am working with OpenFOAM-1.5.00b-wininst it works correctly with cavity tutorial because icofoam.exe exist in Bin folder but interfoam and also rasinterfoam doesn't exist is there any way to get it for windows ?

best regards

I believe there are a few more recent versions available for Windows. I would suggest Googling it. The other option is to run a virtual machine with Linux on it. This approach ios covered on the OpenFOAM website I believe.

[Josh Yang]

Hey,

I wonder did you solve your problem yet?
I am kind of running into a same issue as yours.

Thanks.

Josh

[vonboett]

Originally Posted by vonboett

Hi Mohammad,

the issue with phase reflection at the outlet appears to several users, and type buoyantPressure; value uniform 0; usually helps. There is a funny effect: could you move your mesh to the negative coordinate quadrant (all vertices have x coordinate < 0) and check what happens at the outlet if you use type outletInlet; outletValue uniform 0; for pressure at the open boundary?

Actually, zeroGradient for pressure at the outlet works best for me.

[cjz]

Hello mgdenno,
I'm wondering if you ever got your simulation to run to completion? I've been working on a similar open channel flow for the past couple of weeks and find my simulation fails part way through. There is a sudden velocity magnitude that is orders of magnitude higher than the previous. I've set cAlpha = 0 but the problem remains. If you've been successful I'd be interested in knowing what combination of fvSolution, fvSchemes, and boundary conditions worked for you.

Thanks for any help you can provide.

[mgdenno]

I think what worked in my case was to initially use:

gradSchemes
{
    default         Gauss linear;
    grad(U)        cellLimited Gauss linear 1; 
}

divSchemes
{
    div(rho*phi,U) Gauss linearUpwindV grad(U);
    div(phi,alpha)  Gauss vanLeer;
    div(phirb,alpha) Gauss interfaceCompression;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div(phi,R)      Gauss upwind;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss upwind;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

Hope that helps.

Matt

[sorockin]

Dear Matthew,

I try to simulate flow in open channel with interFoam.
http://www.cfd-online.com/Forums/ope...interfoam.html
My case is 2D and I used BCs from your working case. But I can't overcome instability that arise at inlet. May be you can help me with advice? Unlike your case I turned off turbulence.

Thank you.
Maxim

[cjz]

Have you tried adjusting cAlpha?

from:

http://www.openfoam.org/docs/user/damBreak.php

The cAlpha keyword is a factor that controls the compression of the interface where: 0 corresponds to no compression; 1 corresponds to conservative compression; and, anything larger than 1, relates to enhanced compression of the interface. We generally recommend a value of 1.0 which is employed in this example.

[sorockin]

My cAlpha=1 was and now. But now I took fvSolushion setting from Matthew and looks like issue is solved.
http://www.cfd-online.com/Forums/ope...tml#post444738

Thank you Matthew!

Maxim

[indy07cz]

Hello foamers,
I have a little question about interfaceCompression divScheme for phirb,alpha. When I use this scheme values of Max(alpha.water) go high to numbers like 1.9-2.2 during simulation and due to I must drastically decrease maxAlphaCo to achieve Max(alpha.water) equal to 1 (then simulation takes long time to compute). If I use linear scheme Max(alpha.water) is very close to 1. Can anybody confirm that and tell me why is this happening? Is it somehow connected with mesh quality? Thanks.

[Saideep]

Not sure about your case study but in short to run interfoam cases you generally need to use very small time steps. Courant number of 0.1 is already too large.

There is "Brackbill number" that determines the time step size for volume of fluid computations. I believe/ never had a problem with "interfaceCompression" for the "artificial compression advection term". Probably your also running into classic "spurious current" problem or "volumeRatio" is too high when you used "snappyHexMesh".

So, need more description from your end!!

[indy07cz]

Well I simulate flow over stepped spillway with flow over 200 cms. Mesh has about 2mil cells, and yes there could be problem in mesh volume ratio because smallest cell is 4.3E-5 cubic meters (around spillway crest) and largest is 2.2E-2. CheckMesh is OK. I use Co and alphaCo equal to 0.6 because of computing time (60 seconds takes 2 days). I now when I decrease Co to something about 0.2 then alpha.water is lets say fine, but 5 seconds of simulation takes 1-2 days and I don't have too much time.

I attached some pics to illustrate problem. You can see when I clip results in paraview by threshold for alpha 0-1 lots of cells are missing mainly near wall surfaces.

So I think that biggest problem is high Co number for this simulation.

So I made some research, and I suppose that problem is fine mesh on surfaces in combination with high Co number. I need lower Co or make mash more coarse. Interesting is when i use linear scheme my p_rgh residuals are higher than residuals with interfaceCompression scheme but Max(alpha.water) is higher with interfaceCompression.

[indy07cz]

Hi, after some simulations I found solution for my problem around boundening alpha.water solutions. Even if I reduced Co my Max(alpha.water) was still above 1. Then I added MULES correction to alpha.water in fvSolution and now everything is fine and solution is bounded. But without it I think high alpha values is signal for large timestep and simulation needs Co reduction!

Now the code looks like this:

"alpha.water.*"
    {
        nAlphaCorr      1;
        nAlphaSubCycles 2; 
        cAlpha          1;

        MULESCorr       yes;  
        nLimiterIter    3;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-8;
        relTol 0;
    }

[jesucitolf]

some tutorial or project of an open water channel with transition
im new in openfoam, i want to learn plss. some normal water channel or with transition pls...thx