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

Low pressure drop with the same model

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 15, 2009, 04:56
Default Low pressure drop with the same model
  #1
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
Dear foamers,

I am simulating on a model, which has already simulated by my professor using StarCD. With the same model and same inlet velocity, my professor's pressure drop is 168Pa. While I use simpleFoam in OF, I could not get converged results, and the simulated pressure drop is only 0.004993Pa.

The fvScheme file is:
***************************
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}
divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) 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;
}
***************************
The fvSolution file is:
***************************
solvers
{
p GAMG
{
tolerance 1e-6;
relTol 0.01;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};
U smoothSolver
{
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-8;
relTol 0.1;
};
k PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};
epsilon PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};
R PBiCG
{
preconditioner DILU;
tolerance 1e-05;
relTol 0.1;
};

nuTilda smoothSolver
{
smoother GaussSeidel;
nSweeps 2;
tolerance 1e-8;
relTol 0.1;
};
}
SIMPLE
{
nNonOrthogonalCorrectors 3;
pRefCell 0;
pRefValue 0;
}
relaxationFactors
{
p 0.3;
U 0.7;
k 0.7;
epsilon 0.7;
R 0.7;
nuTilda 0.7;
}
***************************
The log file is:
***************************
Time = 2.3

smoothSolver: Solving for Ux, Initial residual = 0.0039317624097, Final residual = 0.00028429926006, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.00575887542213, Final residual = 0.000439263248628, No Iterations 4
GAMG: Solving for p, Initial residual = 0.0604334923612, Final residual = 0.000305639970335, No Iterations 5
GAMG: Solving for p, Initial residual = 0.00991415857267, Final residual = 5.86040152799e-05, No Iterations 4
GAMG: Solving for p, Initial residual = 0.00071885457453, Final residual = 5.72054751809e-06, No Iterations 5
GAMG: Solving for p, Initial residual = 0.000126793712278, Final residual = 7.18547241099e-07, No Iterations 5
time step continuity errors : sum local = 3.07898278868e-11, global = -2.00751370042e-14, cumulative = -5.60535949412e-11
ExecutionTime = 1826.51 s ClockTime = 1826 s
***************************

As we could see the residual for U and p is very large, here I use deltaT=1e-02.

I struggle at this model, may I ask if some one could give me some idea for this? Thank you.

Bin
zhoubinwx is offline   Reply With Quote

Old   June 15, 2009, 05:32
Default
  #2
Member
 
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 8
marico is on a distinguished road
Hi,

try changing relaxationFactors:
{
p 0.4;
U 0.6;
...
}

and wait....

Marco
marico is offline   Reply With Quote

Old   June 16, 2009, 02:17
Default
  #3
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
Hi Marco,

Thank you for your attention.

Now I have set in fvSolution file:
************************
relaxationFactors
{
p 0.4;//0.3;
U 0.6;//0.7;
k 0.7;
epsilon 0.7;
R 0.7;
nuTilda 0.7;
}
************************
I still get low pressure drop (0.00904) with simpleFoam solver.
Now the log file is:
************************
Time = 35.43
smoothSolver: Solving for Ux, Initial residual = 0.00203370891239, Final residual = 5.6345388581e-05, No Iterations 4
smoothSolver: Solving for Uy, Initial residual = 0.00356242994235, Final residual = 0.000104210543403, No Iterations 4
GAMG: Solving for p, Initial residual = 0.0364082592636, Final residual = 0.000304828677232, No Iterations 4
GAMG: Solving for p, Initial residual = 0.00478820727082, Final residual = 3.86452241619e-05, No Iterations 4
GAMG: Solving for p, Initial residual = 0.000463156930012, Final residual = 2.50732060428e-06, No Iterations 6
GAMG: Solving for p, Initial residual = 7.89315428925e-05, Final residual = 6.66690439345e-07, No Iterations 4
time step continuity errors : sum local = 2.59918498834e-11, global = -2.10847262229e-14, cumulative = -3.47871725926e-12
ExecutionTime = 19303.1 s ClockTime = 19303 s
************************
Now I post my checkMesh log here, I wonder if the mesh quality of fine enough.
************************
Checking geometry...
Overall domain bounding box (-120 0 -0.007) (470 20.001 0.0046667)
Mesh (non-empty) directions (1 1 0)
Mesh (non-empty, non-wedge) dimensions 2
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (5.40237466474e-20 -4.34269087253e-18 -1.95015090065e-14) OK.
Max cell openness = 3.18619574257e-16 OK.
Max aspect ratio = 80.0001195999 OK.
Minumum face area = 3.10546639285e-05. Maximum face area = 0.0736848781216. Face area magnitudes OK.
Min volume = 3.62305447655e-07. Max volume = 0.000859659367582. Total volume = 130.215018482. Cell volumes OK.
Mesh non-orthogonality Max: 85.6112588833 average: 6.3947096647
*Number of severely non-orthogonal faces: 15.
Non-orthogonality check OK.
<<Writing 15 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 2.92248322884 OK.
Mesh OK.
************************
Is it because "severely non-orthogonal faces"? I use Gmsh to build my model, with local fine meshing method.

Welcome again for comment.

Bin

Quote:
Originally Posted by marico View Post
Hi,

try changing relaxationFactors:
{
p 0.4;
U 0.6;
...
}

and wait....

Marco
zhoubinwx is offline   Reply With Quote

Old   June 16, 2009, 02:23
Default
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by zhoubinwx View Post
While I use simpleFoam in OF, I could not get converged results, and the simulated pressure drop is only 0.004993Pa.
1. Do you have the same viscosity as the STAR-CD model?
2. Are you sure about the units of pressure 'p', or do they perhaps include the viscosity (since you are using an incompressible solver 'simpleFoam').
3. Is it possible that you have a different scaling (eg, mm vs. m) when you imported the model from STAR-CD?
olesen is offline   Reply With Quote

Old   June 16, 2009, 02:44
Default
  #5
Member
 
Marco Müller
Join Date: Mar 2009
Location: Germany
Posts: 94
Rep Power: 8
marico is on a distinguished road
Hi,

what is about the turbulence model? You seem to use laminar, since there are no turbulence equations solved... Did your Prof also?
And what about the yPlus values? You could check them to see whether your mesh is appropriate for the case with yPlusRAS..

Marco
marico is offline   Reply With Quote

Old   June 16, 2009, 05:10
Default
  #6
Senior Member
 
ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
zhoubinwx is on a distinguished road
Send a message via ICQ to zhoubinwx Send a message via MSN to zhoubinwx Send a message via Skype™ to zhoubinwx
Hi Olesen and Marico,

Thank you for your attention.

1. Do you have the same viscosity as the STAR-CD model?
Ans: I set in the file transportProperties :
nu [0 2 -1 0 0 0 0] 1.51e-05;

2. Are you sure about the units of pressure 'p', or do they perhaps include the viscosity (since you are using an incompressible solver 'simpleFoam').
Ans: in 0/p file, dimension of p is [0 2 -2 0 0 0 0];
I set 0 for internal field and pressure outlet;

3. Is it possible that you have a different scaling (eg, mm vs. m) when you imported the model from STAR-CD?
Ans: ***** This is the reason******

When I check by the sequence of the post, I find that I use mm instead of micrometer when I convert my mesh.

Therefore I didn't check Marco's suggestions, Hi, sorry Marco

Thank you again for your enthusiasm and kindness.

Grazie.

Bin
zhoubinwx 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
simple model, difficult outlet Eric CFX 7 May 23, 2014 08:13
Total and Static Pressure drop Jaggu FLUENT 3 December 9, 2008 07:03
Pressure drop in symmetric models carno FLUENT 2 August 14, 2007 02:01
Does star cd takes reference pressure? monica CD-adapco 1 April 19, 2007 11:26
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 22:02


All times are GMT -4. The time now is 14:26.