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

twoPhaseEulerFoam: sudden crash

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

Like Tree4Likes
  • 1 Post By mnikku
  • 1 Post By geth03
  • 1 Post By Ardali
  • 1 Post By Ardali

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 9, 2016, 22:19
Default twoPhaseEulerFoam: sudden crash
  #1
New Member
 
hcen
Join Date: May 2016
Posts: 2
Rep Power: 0
hcen is on a distinguished road
Hi everyone,

I am a newbie to OpenFoam, and am now trying to simulate a compressed air-water two phase pipe flow.

I've a mesh created from ICEM with only hex cells. The solver have been crashing and I have no clue what is leading to that. The model is pre-filled with water and has one compressed air inlet and two outlets. Below is the message from terminal. Could anyone take a look and give me a few advises? Thx!

Courant Number mean: 0.00344514823 max: 0.102423844
Max Ur Courant Number = 0.809298941
deltaT = 3.73662022e-06
Time = 0.125824067

PIMPLE: iteration 1
MULES: Solving for alpha.air
MULES: Solving for alpha.air
alpha.air volume fraction = 0.0454209699 Min(alpha.air) = 2.97973812e-316 Max(alpha.air) = 1
Constructing momentum equations
smoothSolver: Solving for e.air, Initial residual = 0.000370432209, Final residual = 4.56780784e-09, No Iterations 2
smoothSolver: Solving for e.water, Initial residual = 3.72096286e-07, Final residual = 5.83454128e-11, No Iterations 1
min T.air -51.5335211
min T.water 208.307104
GAMG: Solving for p_rgh, Initial residual = 0.000283639836, Final residual = 1.04823569e-10, No Iterations 2
PIMPLE: iteration 2
MULES: Solving for alpha.air
MULES: Solving for alpha.air
alpha.air volume fraction = 0.0454209586 Min(alpha.air) = -3.97078944e-17 Max(alpha.air) = 1
Constructing momentum equations
[9] #0 Foam::error:rintStack(Foam::Ostream&)[11] #0 Foam::error:rintStack(Foam::Ostream&) at ??:?
[9] #1 Foam::sigFpe::sigHandler(int) at ??:?
[11] #1 Foam::sigFpe::sigHandler(int) at ??:?
[9] #2 ? at ??:?
[11] #2 ? in "/lib/x86_64-linux-gnu/libc.so.6"
[9] #3 ? in "/lib/x86_64-linux-gnu/libc.so.6"
[11] #3 ? in "/lib/x86_64-linux-gnu/libm.so.6"
[9] #4 pow in "/lib/x86_64-linux-gnu/libm.so.6"
[11] #4 pow in "/lib/x86_64-linux-gnu/libm.so.6"
[9] #5 Foam:ow(Foam::Field<double>&, Foam::UList<double> const&, double const&) in "/lib/x86_64-linux-gnu/libm.so.6"
[11] #5 Foam:ow(Foam::Field<double>&, Foam::UList<double> const&, double const&) at ??:?
[9] #6 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:ow<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensioned<double> const&) at ??:?
[9] #7 Foam::dragModels::SchillerNaumann::CdRe() const at ??:?
[11] #6 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:ow<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensioned<double> const&) at ??:?
[9] #8 Foam::dragModel::Ki() const at ??:?
[11] #7 Foam::dragModels::SchillerNaumann::CdRe() const at ??:?
[9] #9 Foam::dragModel::K() const at ??:?
[11] #8 Foam::dragModel::Ki() const at ??:?
[9] #10 Foam::BlendedInterfacialModel<Foam::dragModel>::K( ) const at ??:?
[9] #11 Foam::twoPhaseSystem::Kd() const at ??:?
[11] #9 Foam::dragModel::K() const at ??:?
[11] #10 Foam::BlendedInterfacialModel<Foam::dragModel>::K( ) const at ??:?
[11] #11 Foam::twoPhaseSystem::Kd() const at ??:?
[9] #12 ? at ??:?
[11] #12 at ??:?
[9] #13 __libc_start_main? in "/lib/x86_64-linux-gnu/libc.so.6"
[9] #14 ? at ??:?
[tande-Precision-Tower-7910:08931] *** Process received signal ***
[tande-Precision-Tower-7910:08931] Signal: Floating point exception (8)
[tande-Precision-Tower-7910:08931] Signal code: (-6)
[tande-Precision-Tower-7910:08931] Failing at address: 0x3e8000022e3
[tande-Precision-Tower-7910:08931] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x35250) [0x7f1e66adb250]
[tande-Precision-Tower-7910:08931] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x37) [0x7f1e66adb1c7]
[tande-Precision-Tower-7910:08931] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x35250) [0x7f1e66adb250]
[tande-Precision-Tower-7910:08931] [ 3] /lib/x86_64-linux-gnu/libm.so.6(+0x12f0c) [0x7f1e67099f0c]
[tande-Precision-Tower-7910:08931] [ 4] /lib/x86_64-linux-gnu/libm.so.6(pow+0x1c) [0x7f1e670ab44c]
[tande-Precision-Tower-7910:08931] [ 5] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam3powERNS_5FieldIdEERKNS_5UL istIdEERKd+0x38) [0x7f1e67f03348]
[tande-Precision-Tower-7910:08931] [ 6] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTurbulenceModels.so(_ZN4Foam3powINS _12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14Geometr icFieldIdT_T0_EEEERKS7_RKNS_11dimensionedIdEE+0x28 e) [0x7f1e6befb2ae]
[tande-Precision-Tower-7910:08931] [ 7] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam10dragModels15SchillerNaumann4CdReEv+0x1d0) [0x7f1e6b0634a0]
[tande-Precision-Tower-7910:08931] [ 8] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam9dragModel2KiEv+0x132) [0x7f1e6b02a1f2]
[tande-Precision-Tower-7910:08931] [ 9] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam9dragModel1KEv+0x2e) [0x7f1e6b029ffe]
[tande-Precision-Tower-7910:08931] [10] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTwoPhaseSystem.so(_ZNK4Foam23Blende dInterfacialModelINS_9dragModelEE1KEv+0x4a3) [0x7f1e6b450453]
[tande-Precision-Tower-7910:08931] [11] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTwoPhaseSystem.so(_ZNK4Foam14twoPha seSystem2KdEv+0x32) [0x7f1e6b436042]
[tande-Precision-Tower-7910:08931] [12] twoPhaseEulerFoam() [0x43510b]
[tande-Precision-Tower-7910:08931] [13] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf0) [0x7f1e66ac6ac0]
[tande-Precision-Tower-7910:08931] [14] twoPhaseEulerFoam() [0x4496a9]
[tande-Precision-Tower-7910:08931] *** End of error message ***
at ??:?
[11] #13 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[11] #14 ? at ??:?
[tande-Precision-Tower-7910:08933] *** Process received signal ***
[tande-Precision-Tower-7910:08933] Signal: Floating point exception (8)
[tande-Precision-Tower-7910:08933] Signal code: (-6)
[tande-Precision-Tower-7910:08933] Failing at address: 0x3e8000022e5
[tande-Precision-Tower-7910:08933] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x35250) [0x7fcddfb32250]
[tande-Precision-Tower-7910:08933] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x37) [0x7fcddfb321c7]
[tande-Precision-Tower-7910:08933] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x35250) [0x7fcddfb32250]
[tande-Precision-Tower-7910:08933] [ 3] /lib/x86_64-linux-gnu/libm.so.6(+0x12f0c) [0x7fcde00f0f0c]
[tande-Precision-Tower-7910:08933] [ 4] /lib/x86_64-linux-gnu/libm.so.6(pow+0x1c) [0x7fcde010244c]
[tande-Precision-Tower-7910:08933] [ 5] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam3powERNS_5FieldIdEERKNS_5UL istIdEERKd+0x38) [0x7fcde0f5a348]
[tande-Precision-Tower-7910:08933] [ 6] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTurbulenceModels.so(_ZN4Foam3powINS _12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14Geometr icFieldIdT_T0_EEEERKS7_RKNS_11dimensionedIdEE+0x22 e) [0x7fcde4f5224e]
[tande-Precision-Tower-7910:08933] [ 7] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam10dragModels15SchillerNaumann4CdReEv+0x1d0) [0x7fcde40ba4a0]
[tande-Precision-Tower-7910:08933] [ 8] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam9dragModel2KiEv+0x132) [0x7fcde40811f2]
[tande-Precision-Tower-7910:08933] [ 9] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleEulerianInterfacialModels.so(_ZNK4F oam9dragModel1KEv+0x2e) [0x7fcde4080ffe]
[tande-Precision-Tower-7910:08933] [10] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTwoPhaseSystem.so(_ZNK4Foam23Blende dInterfacialModelINS_9dragModelEE1KEv+0x4a3) [0x7fcde44a7453]
[tande-Precision-Tower-7910:08933] [11] /home/tande/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64GccDPInt32Opt/lib/libcompressibleTwoPhaseSystem.so(_ZNK4Foam14twoPha seSystem2KdEv+0x32) [0x7fcde448d042]
[tande-Precision-Tower-7910:08933] [12] twoPhaseEulerFoam() [0x43510b]
[tande-Precision-Tower-7910:08933] [13] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xf0) [0x7fcddfb1dac0]
[tande-Precision-Tower-7910:08933] [14] twoPhaseEulerFoam() [0x4496a9]
[tande-Precision-Tower-7910:08933] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 9 with PID 8931 on node tande-Precision-Tower-7910 exited on signal 8 (Floating point exception).

Everything seemed fine to me. The residuals are small, reached with only 1 or 2 iterations. I just didn't understand what was causing the problem. Any suggestion would be appreciated!!!

Best,
HC
hcen is offline   Reply With Quote

Old   June 15, 2016, 08:59
Default
  #2
Member
 
Join Date: May 2015
Posts: 34
Rep Power: 7
mnikku is on a distinguished road
Quote:
Originally Posted by hcen View Post
min T.air -51.5335211
min T.water 208.307104
Well, there's your problem. Your energy equation is probably not converging since you manage to get minus Kelvins. Reasons for this (from my experience) are related to boundary conditions, thought something else might cause this too.
mnikku is offline   Reply With Quote

Old   June 15, 2016, 14:06
Default
  #3
New Member
 
hcen
Join Date: May 2016
Posts: 2
Rep Power: 0
hcen is on a distinguished road
Quote:
Originally Posted by mnikku View Post
Well, there's your problem. Your energy equation is probably not converging since you manage to get minus Kelvins. Reasons for this (from my experience) are related to boundary conditions, thought something else might cause this too.
Thanks man! I developed my set of boundary conditions from the tutorial Bubble Column. For
alpha air : fixed value - inlet; inletoutlet - outlet; zerogradient - walls;
p_rgh: fixedFluxPressure - inlet; totalPressure - outlet; zerogradient - walls;
T: fixedValue - inlet; inletOutlet - outlet; zerogradient - walls;
U_air: flowRateInletVelocity - inlet; pressureInletOutletVelocity - outlet;

The rest of parameters are pretty much the same as the tutorial. I just couldn't figure out what might be the problem. Would you be able to take a look at it? Much appreciated!

Best,
HCen
hcen is offline   Reply With Quote

Old   June 16, 2016, 01:54
Default
  #4
Member
 
Join Date: May 2015
Posts: 34
Rep Power: 7
mnikku is on a distinguished road
You should post some more information about your case for anyone to be able to help you further.
You could test your case with the bubble column boundary conditions if those work with your case.
mnikku is offline   Reply With Quote

Old   June 16, 2016, 10:02
Default
  #5
New Member
 
mohsen ari.
Join Date: Apr 2013
Posts: 12
Rep Power: 10
arianam is on a distinguished road
As mentioned above, the solution diverging. If you keep the track of pressure(e.g. min(p)) , the constant decrease or increase in pressure should be observed.
I should warn you that twoPhaseEulerFoam solver diverges easily if you do not keep your CO and maxdeltaT low enough.
My suggestions:
1. check if you do correctly setFields
2. Lower your CO and maxDeltaT in system/controlDict (e.g. CO to 0.1 and maxDeltaT to 1e-4)
3. Try to under-relax your iteration ( system/fvSolution relaxationFactors)
Hope this might help you!
M. Ariana
arianam is offline   Reply With Quote

Old   October 5, 2016, 03:27
Default
  #6
New Member
 
rakesh927's Avatar
 
rakesh
Join Date: Jul 2015
Location: Nagpur, India
Posts: 16
Rep Power: 7
rakesh927 is on a distinguished road
Quote:
Originally Posted by arianam View Post
As mentioned above, the solution diverging. If you keep the track of pressure(e.g. min(p)) , the constant decrease or increase in pressure should be observed.
I should warn you that twoPhaseEulerFoam solver diverges easily if you do not keep your CO and maxdeltaT low enough.
My suggestions:
1. check if you do correctly setFields
2. Lower your CO and maxDeltaT in system/controlDict (e.g. CO to 0.1 and maxDeltaT to 1e-4)
3. Try to under-relax your iteration ( system/fvSolution relaxationFactors)
Hope this might help you!
M. Ariana
Hi friends,

I am also having similar problem, where twoPhaseEulerFoam crashes after some time. I have found that, before it gets crashed, Max (alpha.air) value jumps inordinately to 1e7 and max. Courant Number is around 8. Although I set maxCo to 0.1 and maxDeltaT to 0.01 is controlDict file.

Awaiting for experts comments.
Thanks
rakesh927 is offline   Reply With Quote

Old   October 5, 2016, 03:31
Default
  #7
Member
 
Join Date: May 2015
Posts: 34
Rep Power: 7
mnikku is on a distinguished road
And the fvSolution? Are you obtaining convergence or just simulation couple of iterations and accepting whatever is the result of that?
mnikku is offline   Reply With Quote

Old   October 5, 2016, 06:45
Default
  #8
New Member
 
rakesh927's Avatar
 
rakesh
Join Date: Jul 2015
Location: Nagpur, India
Posts: 16
Rep Power: 7
rakesh927 is on a distinguished road
Hi,

I am attaching the fvSolution file and convergence plot for p_rgh_0.
Kindly suggest me.
Attached Images
File Type: png 1.png (18.2 KB, 44 views)
Attached Files
File Type: txt fvSolution.txt (2.0 KB, 17 views)
rakesh927 is offline   Reply With Quote

Old   October 5, 2016, 06:55
Default
  #9
Member
 
Join Date: May 2015
Posts: 34
Rep Power: 7
mnikku is on a distinguished road
Please try the search function in these forums, it would have probably found this:
http://www.cfd-online.com/Forums/ope...tml#post607189
mnikku is offline   Reply With Quote

Old   May 5, 2020, 02:05
Default
  #10
New Member
 
sujata
Join Date: Dec 2019
Posts: 10
Rep Power: 3
sujata is on a distinguished road
How did u plot the convergence plot?
sujata is offline   Reply With Quote

Old   May 5, 2020, 02:28
Default
  #11
Member
 
Join Date: May 2015
Posts: 34
Rep Power: 7
mnikku is on a distinguished road
Quote:
Originally Posted by sujata View Post
How did u plot the convergence plot?
You can use whatever plotting tools (Matlab etc) with the logged residual data. In you controlDict, inside functions you have to add

Code:
#includeFunc  residuals
In the system -folder add file residuals, where you specify what residuals to log. These are logged to folder postProcessing/residuals/<starting time step>/residuals.dat . Use this file for plotting.

See User's Guide section 6.3.4.
sujata likes this.
mnikku is offline   Reply With Quote

Old   May 5, 2020, 03:47
Default
  #12
New Member
 
sujata
Join Date: Dec 2019
Posts: 10
Rep Power: 3
sujata is on a distinguished road
Quote:
Originally Posted by mnikku View Post
You can use whatever plotting tools (Matlab etc) with the logged residual data. In you controlDict, inside functions you have to add

Code:
#includeFunc  residuals
In the system -folder add file residuals, where you specify what residuals to log. These are logged to folder postProcessing/residuals/<starting time step>/residuals.dat . Use this file for plotting.

See User's Guide section 6.3.4.
Thanks for the help, will do that and let you know. So, I am a new OpenFOAM user and trying to solve multiphase flow problem with reactingMultiphaseEulerfoam solver. I want to know how to print the drag, lift forces? I saw that there is some center of rotation (CofR). How do I get the direction? Also, I want to print the Cd and Cl. Please, anyone, help me with that. I am using OpenFoam version 4.1.
sujata is offline   Reply With Quote

Old   May 26, 2020, 05:19
Default
  #13
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 233
Rep Power: 4
geth03 is on a distinguished road
Quote:
Originally Posted by sujata View Post
Thanks for the help, will do that and let you know. So, I am a new OpenFOAM user and trying to solve multiphase flow problem with reactingMultiphaseEulerfoam solver. I want to know how to print the drag, lift forces? I saw that there is some center of rotation (CofR). How do I get the direction? Also, I want to print the Cd and Cl. Please, anyone, help me with that. I am using OpenFoam version 4.1.
i know that for openfoam version 6 and 7, there are functions which try to do that. i would suggest updating your version and then checking out
the functionObjects-directory in applications->solvers->multiphase->reactingEulerFoam.

you should be able to print out the phase forces by adding a function to controlDict:
phaseForces.water
{
type phaseForces;
libs ("libreactingEulerFoamFunctionObjects.so");
writeControl outputTime;
writeInterval 1;
log false;
...
phaseName water;
}
sujata likes this.
geth03 is offline   Reply With Quote

Old   June 11, 2020, 22:47
Default
  #14
Member
 
Ardalan
Join Date: Jul 2012
Location: Toronto, Canada
Posts: 72
Rep Power: 10
Ardali is on a distinguished road
As many people sees this problem, I give short answer to this.
If you do not need energy equation discard it in the solver.

If you need it specify correct boundary conditions in T files.

diameterModel in phaseProperties matters as well.
If comprisibility matters to you a lot, e.g.sonic jet or so on, It will be reflected in p_rgh, therefore it wont be a sudden crash. Anyhow, small courant number in the order of 0.1 may help too.
Good luck
Ardalan
jagan1mohan likes this.
Ardali is offline   Reply With Quote

Old   June 13, 2020, 09:57
Default energy equation
  #15
New Member
 
Jagan Mohan
Join Date: Dec 2019
Location: New York
Posts: 18
Rep Power: 3
jagan1mohan is on a distinguished road
Hello Ardali, I'm using twoPhaseEulerFoam (2PEF) and I do not want to use energy equation as my flow is isothermal and it is incompressible.


1. Can you elaborate a bit more on turning off energy equation in this solver?



I have used 288K for all temperature fields initialization, BCs for both gas and particles but there is an energy transfer and temperature varies from 250 K to 320 K.

Thank you,
Jagan Mohan.
jagan1mohan is offline   Reply With Quote

Old   June 13, 2020, 10:06
Default
  #16
Member
 
Ardalan
Join Date: Jul 2012
Location: Toronto, Canada
Posts: 72
Rep Power: 10
Ardali is on a distinguished road
Quote:
Originally Posted by jagan1mohan View Post
Hello Ardali, I'm using twoPhaseEulerFoam (2PEF) and I do not want to use energy equation as my flow is isothermal and it is incompressible.


1. Can you elaborate a bit more on turning off energy equation in this solver?



I have used 288K for all temperature fields initialization, BCs for both gas and particles but there is an energy transfer and temperature varies from 250 K to 320 K.

Thank you,
Jagan Mohan.

Yes, sure,
there two lines in the twoPhaseEulerFoam which says

#include "EEqns.H"
Only comment those two lines and it works fine.
jagan1mohan likes this.
Ardali is offline   Reply With Quote

Old   June 13, 2020, 10:14
Default
  #17
New Member
 
Jagan Mohan
Join Date: Dec 2019
Location: New York
Posts: 18
Rep Power: 3
jagan1mohan is on a distinguished road
Thank you Ardali, I've commented out following two lines as shown below and recompiling it now.


if (faceMomentum) {
....
// #include "EEqns.H"
....

}
else {
....
// #include "EEqns.H"
....

}


So, now I do not have to include the T.particles and T.air files in 0 directory? Also, could you take a look at my other request on the forum.



twoPhaseEulerFoam inlet velocity


Thank you,
Jagan Mohan.
jagan1mohan is offline   Reply With Quote

Old   September 20, 2020, 06:47
Question Divergence issue in reactingmultiphaseEulerFoam
  #18
New Member
 
sujata
Join Date: Dec 2019
Posts: 10
Rep Power: 3
sujata is on a distinguished road
Hello, foamers

I am using OpenFoam 4.1 and using reactingMultiphaseEulerFoam and using the drag, lift, virtual mass, and turbulent dispersion force. I am time averaging it after 40 s to 80s. But after 75 s it doesn't run anymore and shows the following error. Please help me. I am unable to solve it.

[1] #0 Foam::error:rintStack(Foam::Ostream&) at ??:?
[1] #1 Foam::sigFpe::sigHandler(int) at ??:?
[1] #2 ? in "/lib64/libpthread.so.0"
[1] #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) at ??:?
[1] #4 Foam::tmp<Foam::GeometricField<double, Foam::volMesh> > Foam::sqrt<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::volMesh> > const&) at ??:?
[1] #5 Foam::heatTransferModels::RanzMarshall2::K(double) const at ??:?
[1] #6 Foam::BlendedInterfacialModel<Foam::heatTransferMo del>::K() const at ??:?
[1] #7 Foam::HeatTransferPhaseSystem<Foam::MomentumTransf erPhaseSystem<Foam::multiphaseSystem> >::heatTransfer() const at ??:?
[1] #8 ? at ??:?
[1] #9 __libc_start_main in "/lib64/libc.so.6"
[1] #10 ? at ??:?
sujata is offline   Reply With Quote

Old   September 29, 2020, 03:04
Default
  #19
Senior Member
 
Join Date: Dec 2019
Location: Cologne, Germany
Posts: 233
Rep Power: 4
geth03 is on a distinguished road
Quote:
Originally Posted by sujata View Post
Hello, foamers

I am using OpenFoam 4.1 and using reactingMultiphaseEulerFoam and using the drag, lift, virtual mass, and turbulent dispersion force. I am time averaging it after 40 s to 80s. But after 75 s it doesn't run anymore and shows the following error. Please help me. I am unable to solve it.

[1] #0 Foam::error:rintStack(Foam::Ostream&) at ??:?
[1] #1 Foam::sigFpe::sigHandler(int) at ??:?
[1] #2 ? in "/lib64/libpthread.so.0"
[1] #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) at ??:?
[1] #4 Foam::tmp<Foam::GeometricField<double, Foam::volMesh> > Foam::sqrt<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::volMesh> > const&) at ??:?
[1] #5 Foam::heatTransferModels::RanzMarshall2::K(double) const at ??:?
[1] #6 Foam::BlendedInterfacialModel<Foam::heatTransferMo del>::K() const at ??:?
[1] #7 Foam::HeatTransferPhaseSystem<Foam::MomentumTransf erPhaseSystem<Foam::multiphaseSystem> >::heatTransfer() const at ??:?
[1] #8 ? at ??:?
[1] #9 __libc_start_main in "/lib64/libc.so.6"
[1] #10 ? at ??:?
can you also post the prints just before the error message?
this way i can see at which equation the crash occured.
geth03 is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
twoPhaseEulerFoam - sudden enlargement of circular pipe validation case yanxiang OpenFOAM Running, Solving & CFD 17 November 2, 2018 09:09
Is twoPhaseEulerFoam applicable to 3D cases / delivering erroneous results? ThomasV OpenFOAM 0 November 11, 2013 08:10
Sudden crash MaryBau OpenFOAM 3 October 6, 2013 14:13
Sudden crash caused by k-epsilon vainilreb OpenFOAM Running, Solving & CFD 23 August 20, 2013 15:09
CFX Solver : Sudden crash Hervé CFX 2 June 16, 2008 06:40


All times are GMT -4. The time now is 21:54.