ERCOFTAC Centrifugal Pump with kOmegaSST Model

marcelgt87 · November 7, 2012, 08:48

Hi everyone,

I recently got the ERCOFTAC Centrifugal Pump Validation Test Case to run in OF 2.1.0. Originally this Case uses MRFSimpleFoam and the kEpsilon Turbulence Model. More Info on the Case here.

Now I want to run the same Case using the kOmegaSST Model. Unfortunately I did not yet succeed. The Computation always crashes pretty quickly after about 4 or 5 Iterations.

With the Help of http://turbmodels.larc.nasa.gov/sst.html I assembled the following Boundary Conditions:
(though I'm not really sure if they're correct)

INLET:
k: fixedValue 0.48735 ... $k = \frac{3}{2} U_0^2 I^2$ , with $U_0 = 11.4 \frac{m}{s}$ and

)
nut: calculated 0
omega: fixedValue 4873.5 ... $\omega = \frac {k} {\nu} \cdot \left( \frac{\mu_T}{\mu} \right)^{-1}$ with $\nu = 10^{-5} \frac{m^2}{s}$ and $\frac{\mu_T}{\mu} = 10$
p: zeroGradient
U: surfaceNormalFixedValue -11.4 m/s

OUTLET:
k: zeroGradient
nut: calculated 0
omega: zeroGradient
p: fixedValue 0
U: zeroGradient

ROTOR and STATOR:
k: kqRWallFunction 0 ...

at Wall (right?)
nut: nutkWallFunction 0
omega: omegaWallFunction 12500 ... $\omega = 10 \cdot \frac{6 \nu}{0.075 \cdot \Delta d^2}$ with $\nu = 10^-{5} \frac{m^2}{s}$ .
(I'm not really sure what $\Delta d$ is supposed to be. But since I've seen pretty small values being used for it, I assumed it to be the width of the celllayer next to the wall, which would be around $8 \cdot 10^{-4} m$ in my case. Please correct me if I'm wrong!!!)
p: zeroGradient
U: fixedValue 0

INTERNAL FIELD:
k: 3e-7
nut: 0
omega: 100
p: 0
U: 0

FVSCHEMES:

Code:

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linearUpwind Gauss;
    div(phi,k)      Gauss upwind;
    div(phi,omega)  Gauss upwind;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}

FVSOLUTION:

Code:

solvers
{
    p
    {
        solver           GAMG;
        tolerance        1e-7;
        relTol           0.1;
        smoother         GaussSeidel;
        nPreSweeps       0;
        nPostSweeps      2;
        cacheAgglomeration on;
        agglomerator     faceAreaPair;
        nCellsInCoarsestLevel 10;
        mergeLevels      1;
    }

    "(U|k|omega)"
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
	nSweeps         1;
        tolerance       1e-08;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
}
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        k               0.7;
        "omega.*"     	0.7;
    }
}

cache
{
    grad(U);
}

Like I said, I'm not really sure about the BCs for omega. The other BCs should be fine since they are the same as in the kEpsilon Case.

I already tried playing around with the Relaxation Factors, BCs, etc. No Success yet, any ideas?

Any Help would be appreciated!

marcelgt87 · November 9, 2012, 09:09

Well, I guess that was a lesson I won't forget so soon...

if you look closely at my fvSolutions you see that I have an extra closed curly bracket after the SIMPLE-dictionary. This caused OpenFOAM to ignore the Relaxation Factors completely! OF can be a real bitch sometimes!

I hope this thread can help someone and prevent him from going crazy about why his simulations won't work. ^^

Regards,
Marcel

dogan · November 26, 2012, 10:42

Hello Marcel,
in your previous post, you wrote that you are using OpenFOAM 2.1.0., and you wanted to run ERCOFTAC centrifugal pump test case. I would like to ask you whether you managed to run it with this version of O.F.. Since i know (if i am not wrong), the ERCOFTAC centrifugal pump test case requires GGI algorithm, and only O.F. extended version has this algorithm. I am new in using O.F., and i am also trying to run ERCOFTAC test case, but until now, i am unable to do it, because i don't have the extended version of O.F. so if you managed to run it in any case, can you please let me know how you did it?
thank you very much
Dogan

marcelgt87 · November 26, 2012, 11:57

openfoam 2.1.x has the AMI interface implemented which does pretty much the same as the GGI interface. so no need for a dev- or ext-version. look at the mixervesselAMI2D pimpleDyMFoam-tutorial or here for details.

here are my settings for the steady-state case:

PolyMesh / Boundary File

Code:

7
(
    INLET
    {
        type            patch;
        nFaces          434;
        startFace       184170;
    }
    BLADE_ROT
    {
        type            wall;
        nFaces          1743;
        startFace       184604;
    }
    HUB_SHROUD
    {
        type            empty;
        nFaces          187772;
        startFace       186347;
    }
    AMI_INT
    {
        type            cyclicAMI;
        nFaces          707;
        startFace       374119;
        matchTolerance  0.0001;
        neighbourPatch  AMI_EXT;
        transform       noOrdering;
    }
    AMI_EXT
    {
        type            cyclicAMI;
        nFaces          756;
        startFace       374826;
        matchTolerance  0.0001;
        neighbourPatch  AMI_INT;
        transform       noOrdering;
    }
    OUTLET
    {
        type            patch;
        nFaces          804;
        startFace       375582;
    }
    BLADE_STAT
    {
        type            wall;
        nFaces          2760;
        startFace       376386;
    }
)

Boundary Conditions:

epsilon:

Code:

internalField   uniform 0.1;

boundaryField
{
    INLET
    {
        type            fixedValue;
        value           uniform 138.342;
    }
    BLADE_ROT
    {
        type            epsilonWallFunction;
	value           uniform 0;
    }
    HUB_SHROUD
    {
        type            empty;
    }
    OUTLET
    {
        type            zeroGradient;
    }
    BLADE_STAT
    {
        type            epsilonWallFunction;
	value           uniform 0;
    }
    AMI_INT
    {
	type		cyclicAMI;
	value		$internalField;
    }
    AMI_EXT
    {
	type		cyclicAMI;
	value		$internalField;
    }
}

k

Code:

internalField   uniform 0.1;

boundaryField
{
    INLET
    {
        type            fixedValue;
        value           uniform 0.48735;
    }
    BLADE_ROT
    {
        type            kqRWallFunction;
        value           uniform 0;
    }
    HUB_SHROUD
    {
        type            empty;
    }
    OUTLET
    {
        type            zeroGradient;
    }
    BLADE_STAT
    {
        type            kqRWallFunction;
        value           uniform 0;
    }
    AMI_INT
    {
	type		cyclicAMI;
	value		$internalField;
    }
    AMI_EXT
    {
	type		cyclicAMI;
	value		$internalField;
    }
}

nut

Code:

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            calculated;
        value           uniform 0;
    }
    BLADE_ROT
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
    HUB_SHROUD
    {
        type            empty;
    }
    OUTLET
    {
        type            calculated;
        value           uniform 0;
    }
    BLADE_STAT
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
    AMI_INT
    {
	type		cyclicAMI;
	value		$internalField;
    }
    AMI_EXT
    {
	type		cyclicAMI;
	value		$internalField;
    }
}

p

Code:

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            zeroGradient;
    }
    OUTLET
    {
        type            fixedValue;
	value		uniform 0;
    }
    BLADE_ROT
    {
        type            zeroGradient;
    }
    BLADE_STAT
    {
        type            zeroGradient;
    }
    HUB_SHROUD
    {
        type            empty;
    }
    AMI_INT
    {
	type		cyclicAMI;
	value		$internalField;
    }
    AMI_EXT
    {
	type		cyclicAMI;
	value		$internalField;
    }
}

U

Code:

internalField   uniform (0 0 0);

boundaryField
{
    INLET
    {
        type            surfaceNormalFixedValue;
	refValue	uniform -11.4;
    }
    OUTLET
    {
        type            zeroGradient;
    }
    BLADE_ROT
    {
        type            fixedValue;
        value           uniform (0 0 0);    
    }
    BLADE_STAT
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    HUB_SHROUD
    {
	type		empty;
    }
    AMI_INT
    {
	type		cyclicAMI;
	value		$internalField;
    }
    AMI_EXT
    {
	type		cyclicAMI;
	value		$internalField;
    }
}

FvSchemes:

Code:

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss linearUpwind Gauss;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div(phi,R)      Gauss upwind;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss linear;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
    laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DREff,R) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}

FvSolution:

Code:

solvers
{
    p
    {
        solver          GAMG;
        smoother        GaussSeidel;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;

        tolerance       1e-08;
        relTol          0.05;
    }

    "(U|k|epsilon)"
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
	nSweeps         2;
        tolerance       1e-07;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    fields
    {
        p               0.3;
    }
    equations
    {
        U               0.7;
        k               0.7;
        "epsilon.*"     0.7;
    }
}

cache
{
    grad(U);
}

works like a charm. have fun with it

- marcel

RDD · March 13, 2013, 10:49

Hello everybody,

I´m new using OpenFOAM and I´m really looking forward to study a case of a centrifugal pump solved with MRFSimpleFoam.

Does anybody have a case already done where I can learn how to run the simulation?

Thank you very much.
Remo

November 7, 2012, 08:48	ERCOFTAC Centrifugal Pump with kOmegaSST Model	#1
marcelgt87 New Member Marcel Günter Join Date: Mar 2012 Location: Stuttgart, Germany Posts: 20 Rep Power: 14	Hi everyone, I recently got the ERCOFTAC Centrifugal Pump Validation Test Case to run in OF 2.1.0. Originally this Case uses MRFSimpleFoam and the kEpsilon Turbulence Model. More Info on the Case here. Now I want to run the same Case using the kOmegaSST Model. Unfortunately I did not yet succeed. The Computation always crashes pretty quickly after about 4 or 5 Iterations. With the Help of http://turbmodels.larc.nasa.gov/sst.html I assembled the following Boundary Conditions: (though I'm not really sure if they're correct) INLET: k: fixedValue 0.48735 ... $k = \frac{3}{2} U_0^2 I^2$ , with $U_0 = 11.4 \frac{m}{s}$ and ) nut: calculated 0 omega: fixedValue 4873.5 ... $\omega = \frac {k} {\nu} \cdot \left( \frac{\mu_T}{\mu} \right)^{-1}$ with $\nu = 10^{-5} \frac{m^2}{s}$ and $\frac{\mu_T}{\mu} = 10$ p: zeroGradient U: surfaceNormalFixedValue -11.4 m/s OUTLET: k: zeroGradient nut: calculated 0 omega: zeroGradient p: fixedValue 0 U: zeroGradient ROTOR and STATOR: k: kqRWallFunction 0 ... at Wall (right?) nut: nutkWallFunction 0 omega: omegaWallFunction 12500 ... $\omega = 10 \cdot \frac{6 \nu}{0.075 \cdot \Delta d^2}$ with $\nu = 10^-{5} \frac{m^2}{s}$ . (I'm not really sure what $\Delta d$ is supposed to be. But since I've seen pretty small values being used for it, I assumed it to be the width of the celllayer next to the wall, which would be around $8 \cdot 10^{-4} m$ in my case. Please correct me if I'm wrong!!!) p: zeroGradient U: fixedValue 0 INTERNAL FIELD: k: 3e-7 nut: 0 omega: 100 p: 0 U: 0 FVSCHEMES: Code: ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linearUpwind Gauss; div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((nuEffdev(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } FVSOLUTION: Code: solvers { p { solver GAMG; tolerance 1e-7; relTol 0.1; smoother GaussSeidel; nPreSweeps 0; nPostSweeps 2; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; } "(U\|k\|omega)" { solver smoothSolver; smoother GaussSeidel; nSweeps 1; tolerance 1e-08; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; } } relaxationFactors { fields { p 0.3; } equations { U 0.7; k 0.7; "omega." 0.7; } } cache { grad(U); } Like I said, I'm not really sure about the BCs for omega. The other BCs should be fine since they are the same as in the kEpsilon Case. I already tried playing around with the Relaxation Factors, BCs, etc. No Success yet, any ideas? Any Help would be appreciated!

March 13, 2013, 10:49	Centrifugal pump with MRFSimpleFoam	#5
RDD New Member Join Date: Mar 2013 Posts: 2 Rep Power: 0	Hello everybody, I´m new using OpenFOAM and I´m really looking forward to study a case of a centrifugal pump solved with MRFSimpleFoam. Does anybody have a case already done where I can learn how to run the simulation? Thank you very much. Remo

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Use of k-epsilon and k-omega Models	Jade M	Main CFD Forum	40	January 27, 2023 07:18
Blood Damage Modelling via Particle Tracking in a Centrifugal Heart Pump	scatman	CFX	7	January 8, 2018 00:59
flatplate Turbulent BL flow, OF, kOmegaSST model	nikesh	OpenFOAM Post-Processing	0	October 16, 2012 04:43
centrifugal pump, advice required	amir00251	Main CFD Forum	1	August 20, 2012 12:34
stator-rotor interaction in the centrifugal pump	G.H.Lee	Main CFD Forum	4	May 25, 1999 07:33

November 9, 2012, 09:09		#2
marcelgt87 New Member Marcel Günter Join Date: Mar 2012 Location: Stuttgart, Germany Posts: 20 Rep Power: 14	Well, I guess that was a lesson I won't forget so soon... if you look closely at my fvSolutions you see that I have an extra closed curly bracket after the SIMPLE-dictionary. This caused OpenFOAM to ignore the Relaxation Factors completely! OF can be a real bitch sometimes! I hope this thread can help someone and prevent him from going crazy about why his simulations won't work. ^^ Regards, Marcel

November 26, 2012, 10:42		#3
dogan Member Dogan Join Date: Nov 2012 Location: Bochum/Germany Posts: 42 Rep Power: 13	Hello Marcel, in your previous post, you wrote that you are using OpenFOAM 2.1.0., and you wanted to run ERCOFTAC centrifugal pump test case. I would like to ask you whether you managed to run it with this version of O.F.. Since i know (if i am not wrong), the ERCOFTAC centrifugal pump test case requires GGI algorithm, and only O.F. extended version has this algorithm. I am new in using O.F., and i am also trying to run ERCOFTAC test case, but until now, i am unable to do it, because i don't have the extended version of O.F. so if you managed to run it in any case, can you please let me know how you did it? thank you very much Dogan