
[Sponsors] 
February 9, 2009, 13:51 
Hi everyone
i have calculat

#1 
Senior Member

Hi everyone
i have calculated the performance and internal filed in a centrifugal pump impeller using both OpenFOAM1.5 and ANSYS CFX 11.0, for all calculation i use one mesh(i generated the mesh in ICEMCFD 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 offdesign condtion,and for OpenFoam result are all face one problem(i will show in the table below),here is result of 25%Q<sub>design</sub> 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 1e6; relTol 0.05; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 2; nBottomSweeps 2; cacheAgglomeration false; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; }; tolerance 1e06; relTol 0.01; }; U smoothSolver { smoother GaussSeidel; nSweeps 2; tolerance 1e7; relTol 0.01; }; k PBiCG { preconditioner DILU; tolerance 1e7; relTol 0.1; }; omega PBiCG { preconditioner DILU; tolerance 1e7; 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((1A(U)),p) Gauss linear corrected; laplacian((1A(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 /SSTSAS 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.cfdonline.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: SSTOF1.5 kEpsilonCFX11 SSTCFX11 UNSSTCFX11 SSTSASCFX11 LESCFX11 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 

February 10, 2009, 04:17 
How does the history of differ

#2 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12 
How does the history of different residuals looks like?
Could you put some plots with them? Dragos 

February 10, 2009, 05:25 
here is CFX residuals
http:

#3 
Senior Member

here is CFX residuals


February 10, 2009, 05:48 
Be careful Wayne, the picture

#4 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12 
Be careful Wayne, the picture has to be less than 50kB in size.


February 10, 2009, 08:53 
here is CFX residuals
http:/

#5 
Senior Member

here is CFX residuals


February 10, 2009, 08:54 
here is CFX residuals
http:/

#6 
Senior Member

here is CFX residuals


February 10, 2009, 08:57 
here is CFX residuals
http:/

#7 
Senior Member

here is CFX residuals


February 10, 2009, 09:00 
here is OFSST MRFSimpleFOAM

#8 
Senior Member

here is OFSST MRFSimpleFOAM


February 10, 2009, 09:01 
here is OFSST MRFSimpleFOAM

#9 
Senior Member

here is OFSST MRFSimpleFOAM


February 10, 2009, 09:13 
hehe i am sorry,there may be s

#10 
Senior Member

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

February 10, 2009, 09:40 
Hmm, not a very nice convergen

#11 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12 
Hmm, not a very nice convergence, I would say.
Could you plot some vector and pressure distributions? 

February 10, 2009, 10:03 
http://www.cfdonline.com/Open

#12 
Senior Member



February 10, 2009, 10:06 
Well, the SST model in OpenFOA

#13 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
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. 

February 10, 2009, 10:20 
I take that the presented resu

#14 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12 
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 

February 10, 2009, 10:24 
Haha, have a look at the CFX r

#15 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,789
Rep Power: 22 
Haha, have a look at the CFX resudials: they report RMS (Root Mean Square) of the residual instead of sum magnitude.
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
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

February 10, 2009, 13:58 
Hi Euqenne
thanks for your

#16 
Senior Member

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 loglaw region, but in OpenFOAM SST it seem that use the omega expression just for loglaw 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? 

February 10, 2009, 14:17 
Hi Dragos:
i think the velo

#17 
Senior Member

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 postutilities 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 conditionPart I:Particle Image Velocity(PIV) and Laser Dopper Velocimetry(LDV)meassurement,[J]J.fluid.Eng. 2003,Vol125,p6172. 

February 10, 2009, 14:33 
Hi Hrv:
thanks for your rep

#18 
Senior Member

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 Umoment and Vmoment is stable at level of smaller than 1E4 for RMS,but the that is smaller than 1E3 for MAX. i will post the plot tomorrow, thanks! wayne 

February 10, 2009, 14:40 
If your wall function is wrong

#19 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 13 
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.


February 10, 2009, 15:32 
Hi Euqene
i use the default k

#20 
Senior Member

Hi Euqene
i use the default kOmegaSST in OpenFOAM1.5,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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
analysis of pump flow in ANSYS  prakash  CFX  3  September 10, 2008 06:13 
ANSYS GMSH OpenFOAM  gtg627e  Open Source Meshers: Gmsh, Netgen, CGNS, ...  3  December 21, 2007 04:41 
turbulence model for water pump  Marcio  Main CFD Forum  4  September 3, 2003 09:35 
Water Pump to 10 year old kid  Selina Tracy  Main CFD Forum  1  February 11, 2003 23:19 
CFD Package for Water Pump Design !!!  John Sheng  Main CFD Forum  7  September 4, 2001 09:29 