CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Pressure instabilities at the bottom of the domain (http://www.cfd-online.com/Forums/openfoam/112544-pressure-instabilities-bottom-domain.html)

MaryBau January 30, 2013 15:25

Pressure instabilities at the bottom of the domain
 
2 Attachment(s)
Hi;

I am running a case similar to a half channel flow and I am having problems due to some pressure instabilities that form at the bottom of the domain. The deltaT becomes really really really small and eventually the simulation crashes.

It seems that the pressure instabilities happen at the processors boundaries (see pics). I first used the scotch method to decompose the domain and the pressure instabilities are exactly where several processors meet. I also tried to used the simple method to decompose the domain only in the vertical direction, but I guess since most of my cells are close to the bottom, the decomposition did not yield a "perfect" division of the domain in the vertical direction and I also end up with some (less) pressure instabilities.

Notes:

- I am using pisoFoam (adjustableTime), k-w SST-DES and k-w-DDES.
- Cyclic boundaries (inlet-outlet, front-back), no-slip at the bottom and slip at the top.
- My mesh has really small and refined cells at the bottom (y+~0.3). I am using preservePatches (inlet outlet front back);
- pRefCell is not located at the pressure instabilities.


Any suggestions of what could it be the problem or how can I troubleshot it?

Thanks in advance!!!

doubtsincfd January 31, 2013 10:22

Can you post your files so that we can have a look at it in more details?

MaryBau January 31, 2013 14:55

1 Attachment(s)
Thanks a lot doubtsincfd!

Here are the files.

doubtsincfd January 31, 2013 16:58

Quick question: What are the dimensions of the domain you are trying to simulate? Do you scale your mesh? Otherwise it 3000 m long domain

MaryBau January 31, 2013 17:01

Yes, it is a 3000m long domain.

I am doing atmospheric boundary layer simulations.

MaryBau February 1, 2013 17:35

2 Attachment(s)
Hi again;

I ran the same case, but this time without decomposing it, in a single core.

I still get those "pressure instabilities" (see pics). However, this time, the instabilities happen right at pRefCell.

I also checked the flux over the boundaries and it seems to be correct.

Flux at top = 0m^3/s [0 l/min]
Patch: front found on 1/1 processor(s)
Flux at front = 580.795708m^3/s [34847742.5 l/min]
Patch: back found on 1/1 processor(s)
Flux at back = -580.795708m^3/s [-34847742.5 l/min]
Patch: inlet found on 1/1 processor(s)
Flux at inlet = -1494831.5m^3/s [-8.96898898e+10 l/min]
Patch: outlet found on 1/1 processor(s)
Flux at outlet = 1494831.5m^3/s [8.96898898e+10 l/min]
Patch: bottom found on 1/1 processor(s)
Flux at bottom = 0m^3/s [0 l/min]

Any suggestions? Is this normal?

Thanks!!

MaryBau February 19, 2013 17:19

In case someone is having the same issue, I finally solved this problem. The trick was to modifying the solvers for p AND U in the fvSolution file.

I had GAMG for p which I believe is not good for really elongated cells (?) and PBiCG for the velocity. The pressure instabilities disappear when I changed the solvers to PCG for pressure and smoothSolver for the velocity.

So the solvers in my fvSolution file look like this:

Code:

solvers
{
    p
    {
        solver          PCG;
              preconditioner  DIC;
        tolerance      1e-6;
        relTol          0.01;
        minIter        5;
        // maxIter        100;
    }

    pFinal
    {
        solver          PCG;
              preconditioner  DIC;
        tolerance      1e-6; //-7;
        relTol          0;
        minIter        5;
        // maxIter        100;
    }

    U
    {
        //solver          PBiCG;
        //preconditioner  DILU;
        tolerance        1e-6; //-15;
        relTol          0;
        solver          smoothSolver;
        smoother        GaussSeidel;
        nSweeps        1;
        //maxIter                100;
        minIter        1;
    }
   
    k
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-10;
        relTol          0;
        nSweeps        1;
        //maxIter                100;
        minIter        1;

    }

    omega
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance      1e-10;
        relTol          0;
        nSweeps        1;
        //maxIter                100;
        minIter        1;
    }
}



All times are GMT -4. The time now is 15:40.