CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Water pump OpenFOAM 15 ANSYS CFX 110 comparation

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 9, 2009, 13:51
Default Hi everyone i have calculat
  #1
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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<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 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
waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 04:17
Default How does the history of differ
  #2
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
How does the history of different residuals looks like?
Could you put some plots with them?

Dragos
dmoroian is offline   Reply With Quote

Old   February 10, 2009, 05:25
Default here is CFX residuals http:
  #3
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is CFX residuals


waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 05:48
Default Be careful Wayne, the picture
  #4
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Be careful Wayne, the picture has to be less than 50kB in size.
dmoroian is offline   Reply With Quote

Old   February 10, 2009, 08:53
Default here is CFX residuals http:/
  #5
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is CFX residuals

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 08:54
Default here is CFX residuals http:/
  #6
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is CFX residuals

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 08:57
Default here is CFX residuals http:/
  #7
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is CFX residuals

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 09:00
Default here is OF-SST MRFSimpleFOAM
  #8
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is OF-SST MRFSimpleFOAM

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 09:01
Default here is OF-SST MRFSimpleFOAM
  #9
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
here is OF-SST MRFSimpleFOAM

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 09:13
Default hehe i am sorry,there may be s
  #10
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
hehe i am sorry,there may be some problem with internet connetction in my school.

wayne
waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 09:40
Default Hmm, not a very nice convergen
  #11
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hmm, not a very nice convergence, I would say.
Could you plot some vector and pressure distributions?
dmoroian is offline   Reply With Quote

Old   February 10, 2009, 10:03
Default http://www.cfd-online.com/Open
  #12
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618



waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 10:06
Default Well, the SST model in OpenFOA
  #13
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   February 10, 2009, 10:20
Default I take that the presented resu
  #14
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
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
dmoroian is offline   Reply With Quote

Old   February 10, 2009, 10:24
Default Haha, have a look at the CFX r
  #15
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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
hjasak is offline   Reply With Quote

Old   February 10, 2009, 13:58
Default Hi Euqenne thanks for your
  #16
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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?
waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 14:17
Default Hi Dragos: i think the velo
  #17
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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.

waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 14:33
Default Hi Hrv: thanks for your rep
  #18
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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
waynezw0618 is offline   Reply With Quote

Old   February 10, 2009, 14:40
Default If your wall function is wrong
  #19
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   February 10, 2009, 15:32
Default Hi Euqene i use the default k
  #20
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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
waynezw0618 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 00:53.