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

pressure eq. "converges" after few time steps

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

Like Tree14Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2010, 11:34
Question pressure eq. "converges" after few time steps
  #1
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hi everybody,
weird simpleFoam convergence over here, need your help!
I have a complex pipes geometry, similar to what sketched in the geom.png file. The two main pipes are connected by fans to the outside, which is represented by a spherical domain. Reynolds is around 21000 on the smallest pipe, thus a launderSharmaKE model is applied, using wallfunction to keep low the cell number. In any case, the mesh is not really fine since I first want to evaluate my setup. BC are standard:
  • external domain:
    • U, epsilon, k inletOutlet;
    • p fixedValue 0;
  • pipes:
    • U: fixedValue;
    • epsilon, k wallFunction;
    • p zeroGradient;
fvSchemes is as follow:
Code:
grad         faceMDLimited Gauss linear 0.5;
div         Gauss linearUpwind cellLimited Gauss linear 1;
laplacian   Gauss linear limited 0.5;
while I tried different combinations for fvSolution:
Code:
this is the first one:
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U epsilon k
    {
        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-04;
        relTol          0;
    }
and the second one:
Code:
   p
    {
        solver          GAMG;
        tolerance       1e-6;
        relTol          1e-3;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-4;
        relTol          1e-3;
    }
    
    k epsilon
    {
        solver          smoothSolver;
        smoother    GaussSeidel;
        tolerance       1e-4;
        relTol          1e-3;
    }
I ended up with this log file:
Code:
Time = 1

smoothSolver:  Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0    //correct, I applied two fans!
smoothSolver:  Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
GAMG:  Solving for p, Initial residual = 1, Final residual = 9.59218e-07, No Iterations 393
GAMG:  Solving for p, Initial residual = 9.29457e-08, Final residual = 9.29457e-08, No Iterations 0
GAMG:  Solving for p, Initial residual = 9.29457e-08, Final residual = 9.29457e-08, No Iterations 0
time step continuity errors : sum local = 0.00122424, global = -1.32307e-12, cumulative = -1.32307e-12
smoothSolver:  Solving for epsilon, Initial residual = 0.454767, Final residual = 9.2459e-06, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 7.38315e-05, No Iterations 1
ExecutionTime = 174.05 s  ClockTime = 175 s

Time = 2

smoothSolver:  Solving for Ux, Initial residual = 0.141374, Final residual = 5.00021e-05, No Iterations 5
smoothSolver:  Solving for Uy, Initial residual = 0.272753, Final residual = 7.82825e-05, No Iterations 5
smoothSolver:  Solving for Uz, Initial residual = 0.202637, Final residual = 8.15781e-05, No Iterations 5
GAMG:  Solving for p, Initial residual = 8.8497e-08, Final residual = 8.8497e-08, No Iterations 0
GAMG:  Solving for p, Initial residual = 8.8497e-08, Final residual = 8.8497e-08, No Iterations 0
GAMG:  Solving for p, Initial residual = 8.8497e-08, Final residual = 8.8497e-08, No Iterations 0
time step continuity errors : sum local = 0.000634968, global = 7.45987e-07, cumulative = 7.45986e-07
smoothSolver:  Solving for epsilon, Initial residual = 0.164053, Final residual = 2.52305e-06, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 0.24006, Final residual = 1.351e-05, No Iterations 1
ExecutionTime = 192.39 s  ClockTime = 194 s
Does this implies that the pressure is already converged at the second time step???
This does not change when:
- reducing the nNonOrthogonalCorrectors;
- using the second fvSchemes files;
- switching off the turbulence.

Any explanation on that? Really no ideas...

thank you!

maddalena
Attached Images
File Type: jpg geom.jpg (14.3 KB, 356 views)
maddalena is offline   Reply With Quote

Old   October 27, 2010, 12:00
Default
  #2
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 9
FelixL is on a distinguished road
Hi,


try lowering the tolerances of the linear solvers. Something in the order of 1e-12 might be appropriate.

Remember, your simulation is not converged if the residuals of just one equation fall below a certain tolerance. The pressure field depends on the velocity field and vice versa - since your velocity field clearly hasn't converged after the second iteration your whole problem hasn't (would be very surprising if it had) and the pressure equation might and probably will be re-solved at some point.


Greetings,
Felix.
FelixL is offline   Reply With Quote

Old   October 28, 2010, 06:48
Default
  #3
Member
 
Franco Marra
Join Date: Mar 2009
Location: Napoli - Italy
Posts: 52
Rep Power: 8
francescomarra is on a distinguished road
Dear Maddalena,

I would try also changing the initial conditions: I am not aware of your problem but maybe you can try to force the raising of pressure gradients by assigning non zero values for the velocity in the pipes and zero outside.

Regards,

Franco
francescomarra is offline   Reply With Quote

Old   November 2, 2010, 10:28
Default
  #4
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Thanks Felix and Francesco for your suggestions.
Some observations after some more try:
Quote:
Originally Posted by FelixL View Post
try lowering the tolerances of the linear solvers. Something in the order of 1e-12 might be appropriate.
That helped a lot. Now I have p and U equations that are solved at every time step.
Quote:
Originally Posted by FelixL View Post
The pressure field depends on the velocity field and vice versa - since your velocity field clearly hasn't converged after the second iteration your whole problem hasn't (would be very surprising if it had) and the pressure equation might and probably will be re-solved at some point..
Yes, of course I have a feeling of this. But is it correct to first solve U equation and than, after some time, solve p? Is this not longer than solve all the equations at the same time?
Quote:
Originally Posted by francescomarra View Post
I would try also changing the initial conditions: I am not aware of your problem but maybe you can try to force the raising of pressure gradients by assigning non zero values for the velocity in the pipes and zero outside.
About the boundary conditions I am almost sure that everything is fine, since I have already used this setup in the past. However, you suggest to initialize the pipe field with different velocity values, is this correct? If so, how can I do that?

What I have got up to now is a converging but unstable solution: I have bounding epsilon and k warnings, but a convergent solution till time step 295. After that, the max epsilon and k raise suddently and the solution blows away:
Code:
Time = 295

DILUPBiCG:  Solving for Ux, Initial residual = 0.11505, Final residual = 8.32225e-11, No Iterations 13
DILUPBiCG:  Solving for Uy, Initial residual = 0.934182, Final residual = 7.36365e-11, No Iterations 14
DILUPBiCG:  Solving for Uz, Initial residual = 0.713126, Final residual = 4.13259e-11, No Iterations 13
GAMG:  Solving for p, Initial residual = 1.86515e-09, Final residual = 9.94925e-13, No Iterations 206
GAMG:  Solving for p, Initial residual = 6.88289e-10, Final residual = 7.66889e-13, No Iterations 9
time step continuity errors : sum local = 4.67002e-09, global = 1.51568e-10, cumulative = -2.05894e-08
smoothSolver:  Solving for epsilon, Initial residual = 0.00158922, Final residual = 7.46827e-11, No Iterations 24
bounding epsilon, min: 1.30954e-18 max: 5812.76 average: 93.9024
smoothSolver:  Solving for k, Initial residual = 7.82377e-09, Final residual = 4.92151e-11, No Iterations 5
bounding k, min: 6.82659e-17 max: 14.436 average: 0.424139
ExecutionTime = 65389.8 s  ClockTime = 65515 s

Time = 296

DILUPBiCG:  Solving for Ux, Initial residual = 0.328206, Final residual = 5.57292e-11, No Iterations 33
DILUPBiCG:  Solving for Uy, Initial residual = 0.904646, Final residual = 3.81614e-11, No Iterations 30
DILUPBiCG:  Solving for Uz, Initial residual = 0.678265, Final residual = 3.27509e-11, No Iterations 29
GAMG:  Solving for p, Initial residual = 0.000198723, Final residual = 9.87374e-13, No Iterations 723
GAMG:  Solving for p, Initial residual = 5.88726e-07, Final residual = 9.89924e-13, No Iterations 273
time step continuity errors : sum local = 2.72317e-07, global = -1.44975e-09, cumulative = -2.20392e-08
smoothSolver:  Solving for epsilon, Initial residual = 0.998411, Final residual = 5.92556e-11, No Iterations 35
bounding epsilon, min: 1.30845e-18 max: 7.92429e+07 average: 1496.69
smoothSolver:  Solving for k, Initial residual = 1.39098e-07, Final residual = 5.71729e-11, No Iterations 5
bounding k, min: -2.01645e-14 max: 449863 average: 2.44943
ExecutionTime = 65807.2 s  ClockTime = 65932 s

Time = 297

DILUPBiCG:  Solving for Ux, Initial residual = 0.693738, Final residual = 2.49235e-11, No Iterations 28
DILUPBiCG:  Solving for Uy, Initial residual = 0.745261, Final residual = 2.71405e-11, No Iterations 28
DILUPBiCG:  Solving for Uz, Initial residual = 0.715263, Final residual = 2.6154e-11, No Iterations 28
GAMG:  Solving for p, Initial residual = 1.06952e-05, Final residual = 9.67823e-13, No Iterations 738
GAMG:  Solving for p, Initial residual = 3.03894e-09, Final residual = 9.87472e-13, No Iterations 31
time step continuity errors : sum local = 0.00097431, global = 7.21803e-06, cumulative = 7.196e-06
smoothSolver:  Solving for epsilon, Initial residual = 0.587168, Final residual = 7.92945e-11, No Iterations 18
bounding epsilon, min: 1.56953e-17 max: 9.66762e+12 average: 6.49312e+07
smoothSolver:  Solving for k, Initial residual = 0.00708516, Final residual = 1.51465e-11, No Iterations 11
bounding k, min: -3.00985e-15 max: 3.33247e+10 average: 154254
ExecutionTime = 66136 s  ClockTime = 66261 s

Time = 298

DILUPBiCG:  Solving for Ux, Initial residual = 0.652017, Final residual = 5.22231e-11, No Iterations 23
DILUPBiCG:  Solving for Uy, Initial residual = 0.523133, Final residual = 6.68451e-11, No Iterations 21
DILUPBiCG:  Solving for Uz, Initial residual = 0.677302, Final residual = 8.86501e-11, No Iterations 22
GAMG:  Solving for p, Initial residual = 4.62234e-08, Final residual = 9.77244e-13, No Iterations 566
GAMG:  Solving for p, Initial residual = 2.08294e-10, Final residual = 7.37324e-13, No Iterations 4
time step continuity errors : sum local = 0.0110342, global = 0.000335115, cumulative = 0.000342311
smoothSolver:  Solving for epsilon, Initial residual = 0.00963571, Final residual = 9.99631e-11, No Iterations 26
bounding epsilon, min: -2.55095e-15 max: 2.70603e+18 average: 2.26696e+13
smoothSolver:  Solving for k, Initial residual = 0.00019889, Final residual = 6.88818e-11, No Iterations 21
bounding k, min: -2.62403e-13 max: 6.83816e+11 average: 6.84336e+06
ExecutionTime = 66386.5 s  ClockTime = 66512 s
I tried to reduce relaxation (till 0.3 on U, epsilon and k and 0.15 on p) and switch to upwind. No way. The weird thing is that the solution looks good at time 295!
Ideas?

maddalena
maysmech likes this.
maddalena is offline   Reply With Quote

Old   November 2, 2010, 10:34
Default
  #5
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
You could look at the individual cell residuals? That might help you figure out what's causing the instability.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 2, 2010, 10:40
Default
  #6
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by l_r_mcglashan View Post
You could look at the individual cell residuals?
That sounds interesting. How can I do that?
maddalena is offline   Reply With Quote

Old   November 2, 2010, 10:43
Default
  #7
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
I need to do it myself and am just about to look into it

You can jump ahead here:
Local residuals
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 2, 2010, 10:53
Default
  #8
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by l_r_mcglashan View Post
I need to do it myself and am just about to look into it
Ok, so you need a workmate! I will look into it as well.
Stay in touch.

mad
maddalena is offline   Reply With Quote

Old   November 2, 2010, 12:04
Default
  #9
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by l_r_mcglashan View Post
You could look at the individual cell residuals
Done. I modified the simpleFoamResidual utility that hrvoje posted in order to match the new turbulence definition. What I get is a plot showing that the uResidual are higher at the corners of my pipe geometry, thus on the points where the flow is more difficult to model. Does this mean that my mesh is not fine enough on those points?


mad
maddalena is offline   Reply With Quote

Old   November 2, 2010, 12:09
Default
  #10
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
Same. Popped it up on github:

http://github.com/lrm29/OpenFOAM.loc...dualCalculator

OpenFOAM-1.7.x has some errorEstimation libraries which would be nice to use. The residual that simpleFoamResidual calculates needs to be normalised (by the initial state possibly?) so that the changes from step to step can be seen more clearly.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   November 2, 2010, 13:08
Default
  #11
Senior Member
 
Laurence R. McGlashan
Join Date: Mar 2009
Posts: 370
Rep Power: 14
l_r_mcglashan will become famous soon enough
Quote:
Originally Posted by maddalena View Post
What I get is a plot showing that the uResidual are higher at the corners of my pipe geometry, thus on the points where the flow is more difficult to model. Does this mean that my mesh is not fine enough on those points?
Were the residuals increasing in those areas? It's difficult to say, there are a number of problems it could be related to. Versteeg and Malalasekera's book has a nice chapter on possible causes of problems.

Another thing that may be worth checking is that the mass flow into and out of your domain matches.
__________________
Laurence R. McGlashan :: Website
l_r_mcglashan is offline   Reply With Quote

Old   December 2, 2010, 11:11
Default Why my solutiion is not converging?
  #12
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hello,
still here with the same problem on a different case: pressure & velocity fields look good and their residual's trend is "converging"; however local value of residuals (simpleFoamResidual) does not looks good and I have weird oscillations on the initial residual of every time step.
My mesh (tet mesh with no boundary layer) is nice. I have tried tons of different BC-fvSchemes-fvSolution settings. No way.
May this be due to the high number of cyclic patches I am using? Two fans BC + cyclic sides.
I do not what to think now. Suggestions?

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 04:33
Default Reversed problem!
  #13
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Ok, maybe this is not the right place where to post, but I hope to get some answer on a problem that is similar to what posted above...
I started this thread speaking of a pressure equation that converges too soon... And I am writing now for a pressure equation that is never solved within the 1000 iterations of a time step! Geometry and bc are similar to what described above, only the pipe geometry is a little bit more complex than what sketched. Check mesh does not complain about that:
Code:
    Overall domain bounding box (-37.4532 -6.70564 -3.99289e-17) (42.605 6.70578 27.2094)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-2.78883e-18 -1.17153e-15 -2.36782e-14) OK.
    Max cell openness = 3.29759e-16 OK.
    Max aspect ratio = 42.4261 OK.
    Minumum face area = 1.27273e-06. Maximum face area = 9.60387.  Face area magnitudes OK.
    Min volume = 1.12921e-09. Max volume = 8.07969.  Total volume = 9723.47.  Cell volumes OK.
    Mesh non-orthogonality Max: 69.699 average: 18.046
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.956692 OK
.
fvSchemes and fvSolution are:
Code:
grad         faceMDLimited Gauss linear 0.5;
div         Gauss linearUpwind cellLimited Gauss linear 1;
laplacian   Gauss linear limited 0.5;
Code:
p
    {
        solver          GAMG;
        tolerance       1e-10;
        relTol          0;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 10;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    U
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-08;
        relTol          0;
    }
    
    k epsilon
    {
        solver          smoothSolver;
        smoother    GaussSeidel;
        tolerance       1e-08;
        relTol          0;
    }
nNonOrthogonalCorrectors 3;
relaxationFactors
    p: 0.15;
    U, k, epsilon: 0.3;
and this is my weird log.simpleFoam file:
Code:
DILUPBiCG:  Solving for Ux, Initial residual = 0.0028965, Final residual = 2.16561e-11, No Iterations 7
DILUPBiCG:  Solving for Uy, Initial residual = 0.00286544, Final residual = 2.35329e-11, No Iterations 7
DILUPBiCG:  Solving for Uz, Initial residual = 0.00271231, Final residual = 2.42359e-11, No Iterations 7
GAMG:  Solving for p, Initial residual = 0.127338, Final residual = 7.19827e-06, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.0408166, Final residual = 2.54205e-06, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.0144267, Final residual = 1.11529e-06, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.00831105, Final residual = 1.09388e-07, No Iterations 1000
time step continuity errors : sum local = 8.4358e-08, global = -1.12046e-09, cumulative = 7.57121e-10
smoothSolver:  Solving for epsilon, Initial residual = 0.0201266, Final residual = 4.78163e-11, No Iterations 10
smoothSolver:  Solving for k, Initial residual = 0.00307404, Final residual = 3.2731e-11, No Iterations 10
I am using 4 nonOrthogonalCorrectors in order to try to lower p residuals. However, as you can see, pressure equation does not reaches convergence within the 1000 iterations x 4 of each time step. Of course, velocity, turbulence and pressure solution field are far to be as expected.
What I should do? What to change? I really need a help from you!

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 04:40
Default
  #14
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
maddalena

Are you doing some internal loops?
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   February 7, 2011, 04:42
Default
  #15
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hello,
fastest answer ever!
Quote:
Originally Posted by makaveli_lcf View Post
Are you doing some internal loops?
No, that is standard simpleFoam, thus no internal loop.

mad
maddalena is offline   Reply With Quote

Old   February 7, 2011, 04:44
Default
  #16
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf


could U please post more of your log?
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   February 7, 2011, 04:55
Default
  #17
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Yes, sure. Here it is.
As you can see, something strange happens around time step 17 on Uz. On the contrary, pressure does what explained above.

mad
Attached Files
File Type: txt log.simpleFoam.txt (93.0 KB, 73 views)
maddalena is offline   Reply With Quote

Old   February 7, 2011, 04:58
Default
  #18
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
... and your fvScheme and fvSolution in the studio please)))
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   February 7, 2011, 05:00
Default
  #19
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Quote:
Originally Posted by makaveli_lcf View Post
... and your fvScheme and fvSolution in the studio please)))
Written above. However, I tried different combination of them. The log file posted above refers to these two files.

mad
Attached Files
File Type: txt fvSchemes.txt (1.8 KB, 182 views)
File Type: txt fvSolution.txt (1.8 KB, 136 views)
maddalena is offline   Reply With Quote

Old   February 7, 2011, 05:15
Default
  #20
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Maybe it is worth adding that my mesh is tetra mainly. I used prisms in proximity of fans, for the reason explained here. Also, the answer I get here is a bit worrying. Any experience on the subject?

mad
maddalena is offline   Reply With Quote

Reply

Tags
convergence issues, pipe flow, simplefoam

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
TimeVaryingMappedFixedValue irishdave OpenFOAM Running, Solving & CFD 28 May 28, 2015 13:37
time Step's turbFoam >>> exit mgolbs OpenFOAM Pre-Processing 4 December 8, 2009 04:48
Modeling in micron scale using icoFoam m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19
unsteady calcs in FLUENT Sanjay Padhiar Main CFD Forum 1 March 31, 1999 12:32


All times are GMT -4. The time now is 01:23.