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

--> FOAM FATAL ERROR: Maximum number of iterations exceeded

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   August 2, 2012, 11:12
Default --> FOAM FATAL ERROR: Maximum number of iterations exceeded
  #1
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
hi everybody,

I'm solving free convection in 3D in OpenFOAM. my model is a cubic that its bottom temperature is at 400K and the upper plane is at 300K. the sides are isolated.

I'm using buoyantPimpleFoam and when I ran it the below error appeared:

Code:
--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded

    From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.0.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::hRhoThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#3  Foam::hRhoThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"
#5  __libc_start_main in "/lib/libc.so.6"
#6  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantPimpleFoam"
Aborted
anybody knows what is the source of this error?

Thank you

Last edited by adambarfi; August 2, 2012 at 11:58.
adambarfi is offline   Reply With Quote

Old   August 2, 2012, 12:45
Default
  #2
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 725
Rep Power: 18
mturcios777 will become famous soon enough
The crash occurs because there is no convergence when solving for the temperature from the enthalpy using the hConst species thermo model. Have a look at the following thread for some insight into what is happening:

Declaration of function TH()

As for how to fix it, have a look at your enthalpy values and see what they are doing. It could be failing for any number of reasons:

Newton's Method - Failure Analysis

How many iterations have you run when it crahes? Do you notice anything odd about the temperature? Make your write interval smaller to try and see where the problems occur.
mturcios777 is offline   Reply With Quote

Old   August 2, 2012, 13:54
Default
  #3
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by mturcios777 View Post
The crash occurs because there is no convergence when solving for the temperature from the enthalpy using the hConst species thermo model. Have a look at the following thread for some insight into what is happening:

Declaration of function TH()

As for how to fix it, have a look at your enthalpy values and see what they are doing. It could be failing for any number of reasons:

Newton's Method - Failure Analysis

How many iterations have you run when it crahes? Do you notice anything odd about the temperature? Make your write interval smaller to try and see where the problems occur.
Dear Marco,
Thank you for your reply.
this is the full results:

Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.0.1-51f1de99a4bc
Exec   : buoyantSimpleFoam
Date   : Aug 02 2012
Time   : 22:15:47
Host   : mostafa-desktop
PID    : 2069
Case   : /home/mostafa/OpenFOAM/mostafa-2.0.1/run/tutorials/heatTransfer/buoyantSimpleFoam/hotRoom
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


Reading g
Reading thermophysical properties

Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>
Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              -0.33;
    sigmak          1;
    sigmaEps        1.3;
    Prt             1;
}

Calculating field g.h

Reading field p_rgh


SIMPLE: convergence criteria
    field p_rgh     tolerance 0.01
    field U     tolerance 0.001
    field h     tolerance 0.001
    field "(k|epsilon|omega)"     tolerance 0.001


Starting time loop

Time = 1

DILUPBiCG:  Solving for Ux, Initial residual = 0.995791, Final residual = 0.0952429, No Iterations 15
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.06838, No Iterations 30
DILUPBiCG:  Solving for Uz, Initial residual = 6.30029e-13, Final residual = 6.30029e-13, No Iterations 0
DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.0953589, No Iterations 46
DICPCG:  Solving for p_rgh, Initial residual = 0.999987, Final residual = 0.00846449, No Iterations 70
time step continuity errors : sum local = 3.32469, global = 1.6675e-16, cumulative = 1.6675e-16
rho max/min : 2.09115 0.229763
DILUPBiCG:  Solving for epsilon, Initial residual = 0.881107, Final residual = 0.0484186, No Iterations 20
DILUPBiCG:  Solving for k, Initial residual = 1, Final residual = 0.053242, No Iterations 2
bounding k, min: -0.00328955 max: 561.915 average: 38.5853
ExecutionTime = 1.66 s  ClockTime = 4 s

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.778599, Final residual = 0.0675986, No Iterations 34
DILUPBiCG:  Solving for Uy, Initial residual = 0.707139, Final residual = 0.0665317, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.778599, Final residual = 0.0675986, No Iterations 34
DILUPBiCG:  Solving for h, Initial residual = 0.974791, Final residual = 0.0548783, No Iterations 4
DICPCG:  Solving for p_rgh, Initial residual = 0.995251, Final residual = 0.0099475, No Iterations 24
time step continuity errors : sum local = 618.141, global = -1.12147e-13, cumulative = -1.11981e-13
rho max/min : 897.524 -2804.43
DILUPBiCG:  Solving for epsilon, Initial residual = 0.0118022, Final residual = 0.0118152, No Iterations 1001
bounding epsilon, min: -1.005e+14 max: 8.22138e+13 average: 6.92457e+08
DILUPBiCG:  Solving for k, Initial residual = 1.41234e-07, Final residual = 1.41234e-07, No Iterations 0
ExecutionTime = 6.83 s  ClockTime = 9 s

Time = 3

DILUPBiCG:  Solving for Ux, Initial residual = 0.885872, Final residual = 0.0430187, No Iterations 21
DILUPBiCG:  Solving for Uy, Initial residual = 0.828654, Final residual = 0.0514202, No Iterations 26
DILUPBiCG:  Solving for Uz, Initial residual = 0.887219, Final residual = 0.0527398, No Iterations 21
DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.041242, No Iterations 3
DICPCG:  Solving for p_rgh, Initial residual = 0.999199, Final residual = 9.20109, No Iterations 1001
time step continuity errors : sum local = 3.15157e+11, global = -6.37253e-06, cumulative = -6.37253e-06
rho max/min : 3.06985e+11 -2.33027e+11
DILUPBiCG:  Solving for epsilon, Initial residual = 0.516331, Final residual = 0.0441885, No Iterations 1
bounding epsilon, min: -2.26825e+24 max: 1.63517e+26 average: 3.51799e+21
DILUPBiCG:  Solving for k, Initial residual = 0.981172, Final residual = 0.0828003, No Iterations 1
bounding k, min: -1.60611e+23 max: 4.27903e+27 average: 1.01515e+23
ExecutionTime = 9.48 s  ClockTime = 11 s

Time = 4

DILUPBiCG:  Solving for Ux, Initial residual = 0.909059, Final residual = 0.062452, No Iterations 4
DILUPBiCG:  Solving for Uy, Initial residual = 0.987006, Final residual = 0.0514382, No Iterations 4
DILUPBiCG:  Solving for Uz, Initial residual = 0.967417, Final residual = 0.03232, No Iterations 4
DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.084893, No Iterations 2


--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded

    From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.0.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#3  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
#5  __libc_start_main in "/lib/libc.so.6"
#6  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
Aborted
adambarfi is offline   Reply With Quote

Old   August 2, 2012, 14:00
Default
  #4
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 725
Rep Power: 18
mturcios777 will become famous soon enough
You've got a lot of problems with your case setup; rho, k and epsilon are all blowing up! My guess is that paying more attention to your boundary and initial conditions will solve the issues. Have a look at the tutorial cases and see if your boundary conditions are consistent for walls and open boundaries.
mturcios777 is offline   Reply With Quote

Old   August 2, 2012, 14:33
Default
  #5
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by mturcios777 View Post
You've got a lot of problems with your case setup; rho, k and epsilon are all blowing up! My guess is that paying more attention to your boundary and initial conditions will solve the issues. Have a look at the tutorial cases and see if your boundary conditions are consistent for walls and open boundaries.
Wooow!
Thanks Marco,
I'm trying to solve natural convection in a closed box. in first post I explain it. I check the boundary, they are alright.
I'm so confused! I guess this errors are originated from my meshes. I should check it.
adambarfi is offline   Reply With Quote

Old   August 2, 2012, 15:10
Default
  #6
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
hi
My bottom temperature is 3000K. when I reduce it to 400K there is no error!!! why?!? anybody knows?
adambarfi is offline   Reply With Quote

Old   August 2, 2012, 15:12
Default
  #7
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 725
Rep Power: 18
mturcios777 will become famous soon enough
What do you mean bottom temperature? Bottom of the room, bottom range of interpolation?
mturcios777 is offline   Reply With Quote

Old   August 2, 2012, 16:05
Default
  #8
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by mturcios777 View Post
What do you mean bottom temperature? Bottom of the room, bottom range of interpolation?
sorry, bottom of the room!!! I get results with T=1000K. but It don't work for 3000K!!!!!!!
but I think they aren't true. the convection occurs weakly, but temperature is pretty high!!!!
adambarfi is offline   Reply With Quote

Old   August 2, 2012, 16:39
Default
  #9
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 725
Rep Power: 18
mturcios777 will become famous soon enough
Sounds like its a matter of tweaking the model, maybe selecting a different species thermophysical models. I haven't done much with free convection, so you'll have to ask someone with more experience.
mturcios777 is offline   Reply With Quote

Old   August 2, 2012, 16:46
Default
  #10
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Maybe you can try a lower deltaT in you controlDict file.
Regards
Mojtaba.a is offline   Reply With Quote

Old   August 3, 2012, 03:18
Default
  #11
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by Mojtaba.a View Post
Maybe you can try a lower deltaT in you controlDict file.
Regards
Dear Mojtaba,
I tested it, again the convection was very weak. I solve this geometry with Fluent and it solved it correctly. but I don't understand why the temperature distribution is wrong?!?!?!? actually in my model the convection doesn't occur. the bottom plane remains at T=1000K and the rest remains T=300.

do you know what is wrong?
adambarfi is offline   Reply With Quote

Old   August 3, 2012, 05:56
Default
  #12
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Quote:
Originally Posted by adambarfi View Post
Dear Mojtaba,
I tested it, again the convection was very weak. I solve this geometry with Fluent and it solved it correctly. but I don't understand why the temperature distribution is wrong?!?!?!? actually in my model the convection doesn't occur. the bottom plane remains at T=1000K and the rest remains T=300.

do you know what is wrong?
Dear Mostafa,
I don't have too much experience in free convection. Maybe a person with more knowledge can help you. But i suggest you to have a look at this tutorial by Abolfazl Shiri:

http://www.tfd.chalmers.se/~hani/kur...i/NC_Shiri.pdf

Regards
Mojtaba
Mojtaba.a is offline   Reply With Quote

Old   August 5, 2012, 06:45
Default
  #13
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
hi everybody,

again this error appears:

Code:
--> FOAM FATAL ERROR: 
Maximum number of iterations exceeded

    From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.0.1/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#3  Foam::hPsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/opt/openfoam201/platforms/linux64GccDPOpt/lib/libbasicThermophysicalModels.so"
#4  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
#5  __libc_start_main in "/lib/libc.so.6"
#6  
 in "/opt/openfoam201/platforms/linux64GccDPOpt/bin/buoyantSimpleFoam"
Aborted
what should I do?!?!? I'm trying just to solve natural convection in a cubic!!!
please Help me
adambarfi is offline   Reply With Quote

Old   August 5, 2012, 11:52
Default
  #14
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Quote:
Originally Posted by adambarfi View Post
what should I do?!?!? I'm trying just to solve natural convection in a cubic!!!
please Help me
Post your residuals plot and your controlDict file to see what happens.
Mojtaba.a is offline   Reply With Quote

Old   August 6, 2012, 03:10
Default
  #15
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by Mojtaba.a View Post
Post your residuals plot and your controlDict file to see what happens.
here you are the contrilDict and log files

thank you Mojtaba
Attached Files
File Type: gz cavity.tar.gz (2.2 KB, 31 views)
adambarfi is offline   Reply With Quote

Old   July 21, 2013, 20:07
Default
  #16
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
I could solve it by defining zeroGradient boundary condition for p and p_rgh
laurentD likes this.
__________________
Complex Heat & Flow Simulation Research Group
If you can't explain it simply, you don't understand it well enough. "Richard Feynman"
Mojtaba.a is offline   Reply With Quote

Old   August 2, 2013, 07:58
Default
  #17
New Member
 
M Bay
Join Date: Jun 2013
Location: Germany
Posts: 10
Rep Power: 4
mbay101 is on a distinguished road
Hi,

I m having the same Problem with my case. I m trying to simulate a constraction in free convection. After the first Time step i get: maximum number of iterations has been exceeded. exact the sameone that Mostafa got.

can i post my case so you expert can take a look in it? because I tried everything and nothing seems to be working . I change the BC, the solver for AIR, the Delta, checkt the initial condition, working with other Relaxations Factores and checkMesh can find no problem with my Mesh.

My porbleme apears when OP calculate h for my Air region. the T value seems to go higher then it should be.

Please Please someone help.

to Mostafa: dose your case work now? can you please post it ?

Regards
mbay101 is offline   Reply With Quote

Old   August 2, 2013, 15:04
Default
  #18
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 233
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Quote:
Originally Posted by mbay101 View Post
Hi,

I m having the same Problem with my case. I m trying to simulate a constraction in free convection. After the first Time step i get: maximum number of iterations has been exceeded. exact the sameone that Mostafa got.

can i post my case so you expert can take a look in it? because I tried everything and nothing seems to be working . I change the BC, the solver for AIR, the Delta, checkt the initial condition, working with other Relaxations Factores and checkMesh can find no problem with my Mesh.

My porbleme apears when OP calculate h for my Air region. the T value seems to go higher then it should be.

Please Please someone help.

to Mostafa: dose your case work now? can you please post it ?

Regards

Maybe you can use some bounded Div schemes in your fvscheme file.
Try to play with different combinations of schemes.

Try to use more bounded ones, instead of more accurate schemes. after some iterations you can change back to second order and unbounded schemes for more accuracy.

best
__________________
Complex Heat & Flow Simulation Research Group
If you can't explain it simply, you don't understand it well enough. "Richard Feynman"
Mojtaba.a is offline   Reply With Quote

Old   August 5, 2013, 10:12
Default
  #19
New Member
 
M Bay
Join Date: Jun 2013
Location: Germany
Posts: 10
Rep Power: 4
mbay101 is on a distinguished road
Hi Mojtaba,

sorry for the comend queation but i m new in OpenFoam.
what do you mean with more bounded div schemes? I m using bounded Gauss upwind for all of my div schemes. Only for div(R) and div((muEff*... i m using Gauss linear.

thank you
Best Regards
mbay101 is offline   Reply With Quote

Old   December 5, 2014, 13:31
Default
  #20
New Member
 
Join Date: Nov 2014
Posts: 11
Rep Power: 2
slash89 is on a distinguished road
Hi all,
i got the same problem. I am using the buoyantSimpleRadiationFoam. The problems is always at the second time step, when solving the G file. Any suggestions to fix this problem?

Thank you,

Best regards
slash89 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
simpleFoam error - "Floating point exception" mbcx4jc2 OpenFOAM Running, Solving & CFD 11 June 25, 2015 13:53
Decomposing meshes Tobi OpenFOAM Pre-Processing 1 September 9, 2014 05:30
SixDoFRigidBodyMotion under OF2.3 ( self oscillating cylinder) Scabbard OpenFOAM Running, Solving & CFD 1 July 22, 2014 04:50
pisoFoam with k-epsilon turb blows up - Some questions Heroic OpenFOAM Running, Solving & CFD 26 December 17, 2012 04:34
High Courant Number @ icoFoam Artex85 OpenFOAM Running, Solving & CFD 9 January 3, 2012 09:06


All times are GMT -4. The time now is 06:56.