Hi everyone i have calculat
 

Hi everyone

i have calculated the performance and internal filed in a centrifugal pump impeller using both OpenFOAM-1.5 and ANSYS CFX 11.0, for all calculation i use one mesh(i generated the mesh in ICEM-CFD 11.0,save a copy as .cfx for CFX,and the other as .msh for OpenFOAM,so for both solver use the same mesh)

the working conditions of all simulations are all part load off-design condtion,and for OpenFoam result are all face one problem(i will show in the table below),here is result of 25%Q_design

in OpenFOAM i have use both simpleSRFFoam & MRFSimpleFoam,and turbulence model is SST,the both two get the similar result,so i will show the result of MRFSimpleFoam here only ,here is fvScheme and fvSolution for MRFSimpleFoam

fvSolution:

solvers
{
p PCG
{
preconditioner GAMG
{

tolerance 1e-6;
relTol 0.05;

smoother DICGaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nBottomSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;

};
tolerance 1e-06;
relTol 0.01;
};
U smoothSolver
{
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-7;
relTol 0.01;
};
k PBiCG
{
preconditioner DILU;
tolerance 1e-7;
relTol 0.1;
};
omega PBiCG
{
preconditioner DILU;
tolerance 1e-7;
relTol 0.1;
};
}

SIMPLE
{
nNonOrthogonalCorrectors 2;
}

relaxationFactors
{
p 0.3;
U 0.4;
k 0.4;
omega 0.4;
}


!! nNonOrthogonalCorrectors is 2

fvScheme:

ddtSchemes
{
default steadyState;
}

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

}

divSchemes
{
default none;
div(phi,U) Gauss SFCD;
div(phi,Urel) Gauss SFCD;
div(phi,k) Gauss linear;
div(phi,epsilon) Gauss linear;
div(phi,omega) Gauss linear;
div(phi,v2) Gauss limitedLinear 0.5;
div(phi,f) Gauss limitedLinear 0.5;
div(phi,R) Gauss linear;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
div((nuEff*dev(grad(Urel).T()))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
laplacian(nuEff,U) Gauss linear corrected;
laplacian(nuEff,Urel) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
laplacian((1|A(Urel)),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DomegaEff,omega) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

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

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

in CFX i try to use the StandardkEpsilo+scable wallfunction
/SST+ automatic wall fuction
/unsteady SST+automatic wall fuction
/SST-SAS automatic wall fuction
/LES Smaginsky subgrid model + scalable wall function

and the advection term scheme is High Resoltion method in ANSYS CFX11.0

the result of internel field is almost the same for all OF and CFX(I have post before:http://www.cfd-online.com/OpenFOAM_D...es/1/9426.html)

the stange thing is in openFOAM the pressure torque on Blade is very small(!!more than 10% of that of CFX SST),you could see in the table below:



SST-OF1.5 kEpsilon-CFX11 SST-CFX11 UNSST-CFX11 SSTSAS-CFX11 LES-CFX11

Torque_p@blade 0.39 0.41 0.43 0.43 0.44 0.45

Torque_viscous@blade 0.0039 0.0031 0.0035 0.0035 0.0036 0.0038

Torque_viscous@hub 0.054 0.012 0.015 0.015 0.018 0.049

Torque_viscous@shroud 0.053 0.020 0.030 0.033 0.033 0.048




i don`t know why but i guess there maybe 2 problems:

1) in fvScheme and fvSolutin. the scheme is different for CFX and OpenFOAM
2) solver.for ANSYS CFX is coupled solver for p and U,but NOT in OF

or is there any other things will cause the differents?

how can i resolve it ? how to set the fvScheme(to to switch on some limiters ) and fvSolution(change for p???) ??

thanks

yours wayne

How does the history of differ
 

How does the history of different residuals looks like?
Could you put some plots with them?

Dragos

here is CFX residuals http:
 

here is CFX residuals

http://www.cfd-online.com/OpenFOAM_D...your_image.gif

Be careful Wayne, the picture
 

Be careful Wayne, the picture has to be less than 50kB in size.

here is CFX residuals http:/
 

here is CFX residuals
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

here is CFX residuals http:/
 

here is CFX residuals
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

here is CFX residuals http:/
 

here is CFX residuals
http://www.cfd-online.com/OpenFOAM_D...es/1/11070.png

here is OF-SST MRFSimpleFOAM
 

here is OF-SST MRFSimpleFOAM
http://www.cfd-online.com/OpenFOAM_D...your_image.gif

here is OF-SST MRFSimpleFOAM
 

here is OF-SST MRFSimpleFOAM
http://www.cfd-online.com/OpenFOAM_D...es/1/11073.jpg

hehe i am sorry,there may be s
 

hehe i am sorry,there may be some problem with internet connetction in my school.

wayne

Hmm, not a very nice convergen
 

Hmm, not a very nice convergence, I would say.
Could you plot some vector and pressure distributions?

http://www.cfd-online.com/Open
 

http://www.cfd-online.com/OpenFOAM_D...es/1/11075.jpg

http://www.cfd-online.com/OpenFOAM_D...es/1/11076.jpg

Well, the SST model in OpenFOA
 

Well, the SST model in OpenFOAM does not use scalable wall functions. That could make a very big difference to the shear stress depending on y+.

To compare with the FOAM models, you will have to run standard wall functions.

Also, SFCD is a very diffusive scheme. I suggest something like linearUpwind, limitedLinear or Gamma.

I take that the presented resu
 

I take that the presented results are OpenFOAM.
The pressure distribution looks uniform, but the velocity distribution... Did you expect to have such a different flow in almost every channel?
Another thing is that your vectors seem to show the relative velocity, could you post the same picture using the absolute velocity instead? Use the OpenFOAM results.

Dragos

Haha, have a look at the CFX r
 

Haha, have a look at the CFX resudials: they report RMS (Root Mean Square) of the residual instead of sum magnitude. http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

This is laughable: the residual plot of this kind carries no meaning. Switch to proper residual formulation and you will find that your CFX run is nowhere near convergence.

Hrv

Hi Euqenne thanks for your
 

Hi Euqenne

thanks for your reply,i will try limtedLinear later

in CFX the wall function for SST is not scalable wall function, it is "automatic near wall treatment". and it calculate the omega in analytical expression for viscous sublayer and log-law region, but in OpenFOAM SST it seem that use the omega expression just for log-law region,and also the production ternm G has some different from ANSYS CFX.

so i can understand the different for viscous torque.

my problem is what cause the pressure torque different for blade? and the different is so large?

Hi Dragos: i think the velo
 

Hi Dragos:

i think the velocity distribution in such working condition is something you have seen in the picture.the geometry information of impeller and pump working conditon is come from a reference paper.in the reference paper,the velocity distribution is gotten from PIV and LDV,also LES,and the picture i have post here is the same as in the paper(the CFX SST result is also something like that!).

anyway the vectors picture is OpenFOAM result,and it is relative velocity.and i have write a post-utilities to convert the absolute velocity to relative velocity. and i think it could see the flow separation more clearly in the channels.and i will post the absolute one tomorrow,for i am out of office now,please tell me more.

thanks

wayne


reference paper:

[1]Nicolas Perdeson,etc.Flow in a Centrifugal pump impeller at design and off design condition-Part I:Particle Image Velocity(PIV) and Laser Dopper Velocimetry(LDV)meassurement,[J]J.fluid.Eng. 2003,Vol125,p61-72.

Hi Hrv: thanks for your rep
 

Hi Hrv:

thanks for your reply.

and i also have a max of residual plot,the profile of max residual plot is similar to the RMS one,but the value will be larger,for example the U-moment and V-moment is stable at level of smaller than 1E-4 for RMS,but the that is smaller than 1E-3 for MAX.

i will post the plot tomorrow,

thanks!

wayne

If your wall function is wrong
 

If your wall function is wrong then it will affect everything, not just the surface shear. For instance, stronger surface shear will keep a boundary layer attached more firmly and strongly affect the pressure due to increase flow curvature.

Hi Euqene i use the default k
 

Hi Euqene
i use the default kOmegaSST in OpenFOAM-1.5,which do have wall function. you could find them in $FOAM_SRC/turbulenceModel/RAS/incompressble/kOmegaSST.

and maybe i will make some comparision for velocity profile?

thanks!

yours wayne