
[Sponsors] 
February 13, 2015, 14:29 
similar problem, but maybe related to some BC

#21 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Greetings all,
I know this is a very old thread but I'm facing a problem that looks very similar to the one posted here. I'm dealing with a multi region case with the chtMultiRegionFoam solver. My case is made up of some solid regions and a fluid region. It starts solving first the fluid region with no problem but when it starts to solve the first solid region the following error comes up: Code:
Solving for solid region fasana #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 in "/lib64/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #4 Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #5 parserPatch::PatchValueExpressionParser::parse() at ??:? #6 Foam::PatchValueExpressionDriver::parseInternal(int) at ??:? #7 Foam::CommonValueExpressionDriver::parse(Foam::exprString const&, Foam::word const&) at ??:? #8 Foam::tmp<Foam::Field<double> > Foam::CommonValueExpressionDriver::evaluate<double>(Foam::exprString const&, bool) at ??:? #9 Foam::groovyBCFvPatchField<double>::updateCoeffs() at ??:? #10 Foam::mixedFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) at ??:? #11 Foam::mixedEnergyFvPatchScalarField::updateCoeffs() at ??:? #12 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoeffs() at ??:? #13 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:? #14 at ??:? #15 at ??:? #16 __libc_start_main in "/lib64/libc.so.6" #17 at /home/abuild/rpmbuild/BUILD/glibc2.17/csu/../sysdeps/x86_64/start.S:126 Code:
Cell determinant (wellposedness) : minimum: 0 average: 3.2312708 ***Cells with small determinant (< 0.001) found, number of cells: 960 <<Writing 960 underdetermined cells to set underdeterminedCells After I solved the problem with the under determined cells I ran the case again but the same error was shown, so I got stuck because I don't know what it really means and I don't know where to look up. I attach the changeDictionaryDict file and the T file belonging to the region that crashes so that you can check if there is something wrong in them. In case you need more files or even the entire case, just ask me for it! Many thanks in advance. Regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

February 14, 2015, 11:49 

#22 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 127 
Greetings Alex,
In a case like this, you should apply the good old strategy of "isolate and conquer". Anyway, from what I can see in the "T" file you provided, there are two major threats:
Bruno
__________________


February 14, 2015, 14:48 

#23  
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Dear Bruno,
Thanks for your quick answer! Quote:
Quote:
Well, now I could finally make it work I still have a problem. The problem is that the simulation starts running but after some time steps it crashes. Here you can see the last time steps for the fluid region (the one that make it crash): Code:
Time = 158 Solving for fluid region cambra_aire diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.43303564, Final residual = 3.1317423e08, No Iterations 7 DILUPBiCG: Solving for Uy, Initial residual = 0.30021911, Final residual = 6.5293486e09, No Iterations 8 DILUPBiCG: Solving for Uz, Initial residual = 0.06714822, Final residual = 1.6341749e08, No Iterations 7 DILUPBiCG: Solving for h, Initial residual = 0.060831265, Final residual = 1.0189158e08, No Iterations 6 Min/max T:16.83129 315.55516 GAMG: Solving for p_rgh, Initial residual = 0.17209656, Final residual = 0.0015065066, No Iterations 2 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (cambra_aire): sum local = 0.018986281, global = 0.0041410354, cumulative = 1.0939806 GAMG: Solving for p_rgh, Initial residual = 0.023029345, Final residual = 9.9287594e08, No Iterations 10 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (cambra_aire): sum local = 1.3786288e06, global = 3.2030593e07, cumulative = 1.0939809 ... Time = 159 Solving for fluid region cambra_aire diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.59164209, Final residual = 2.3456257e08, No Iterations 8 DILUPBiCG: Solving for Uy, Initial residual = 0.56513797, Final residual = 5.357496e08, No Iterations 8 DILUPBiCG: Solving for Uz, Initial residual = 0.29594071, Final residual = 1.6331144e08, No Iterations 8 DILUPBiCG: Solving for h, Initial residual = 0.35403101, Final residual = 1.7882418e08, No Iterations 7 Min/max T:24.990244 315.57784 GAMG: Solving for p_rgh, Initial residual = 0.50051967, Final residual = 0.0038889656, No Iterations 4 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (cambra_aire): sum local = 0.08336456, global = 0.0075688716, cumulative = 1.1015498 GAMG: Solving for p_rgh, Initial residual = 0.033368512, Final residual = 9.248029e08, No Iterations 20 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (cambra_aire): sum local = 2.9077841e06, global = 7.1199841e08, cumulative = 1.1015497 ... Time = 160 Solving for fluid region cambra_aire diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.83563518, Final residual = 1.1467818e08, No Iterations 11 DILUPBiCG: Solving for Uy, Initial residual = 0.7633537, Final residual = 2.8147703e08, No Iterations 12 DILUPBiCG: Solving for Uz, Initial residual = 0.73226472, Final residual = 2.7058083e08, No Iterations 11 DILUPBiCG: Solving for h, Initial residual = 0.96491629, Final residual = 8.0298622e09, No Iterations 12 > FOAM FATAL ERROR: Maximum number of iterations exceeded From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const in file /home/cfd/OpenFOAM/OpenFOAM2.3.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::T(double, double, double, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double, double) const, double (Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::*)(double) const) const at ??:? #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:? #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:? #5 at ??:? #6 __libc_start_main in "/lib64/libc.so.6" #7 at /home/abuild/rpmbuild/BUILD/glibc2.17/csu/../sysdeps/x86_64/start.S:126
For more info, the case is about an air chamber that is heated by the solar radiation and the air inside the chamber flows because of the effect of the convection. If you need more info feel free to ask! If I had more time I would have taken some screenshots so that you could see which cells lead to this crash. I will upload them as soon as I can! Regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

February 14, 2015, 15:00 

#24 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 127 
Hi Alex,
temperatures below 0 Kelvin... It's very much possible that you're triggering an issue related to simulating heat transfer with a steadystate solver. This was addressed sometime ago in another thread... ah, here you go, start reading from here: http://www.cfdonline.com/Forums/ope...tml#post528307 post #60. And yes, the idea I was trying to give you was exactly about having the variable initializations at the top. And C++ is very similar to C, only just very much more organized... if coded correctly And I knew that something wouldn't exactly as intended with changeDictionary I just couldn't remember what it was exactly. Either way, the thread I mentioned hopefully will get you in the right direction. Good luck! Best regards, Bruno 

February 16, 2015, 10:20 

#25 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Hi Bruno,
Thanks for the link but it's not exactly the same problem since my case is a transient one, not steadystate. Now I've had some time I took some screenshots so that you can have an idea about my problem. Here you can see the geometry I used. As you can see the air region is in the front, and the solid regions are just right behind it (the outline can be seen so that you can have an idea of my geometry). Attached you can find the temperature distribution for the last time step before it crashed. Also the U distribution is attached. As it is shown, the problem comes from the cells near the inlet patch, an extremely high velocity going out of the domain leads to an unphysical temperature distribution in the neighbouring cells, at least this is what it seems to my unexperinced eyes in the field of compressible flow in an opened domain... I have tried with different discretizations, with a coarser mesh but it allways crashes, sometimes sooner, sometimes later, but it crashes all the time... I don't know if it is a problem of the mesh or a bad definition of the BC's (specification can be seen some posts above!). I need a little help to find the correct way to make it run. Many thanks in advance. Regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

February 16, 2015, 18:41 

#26  
Senior Member
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 12 
Quote:
moving on ... have you checked that the regions are really conformal? (assuming this not AMI) and you havent gained an extra region? I remember this causing similar issues.
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET 

February 22, 2015, 14:08 

#27 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Hello,
Finally I managed to "solve" it. The problem was, I guessed, the Courant number. The fact is that I was solving the case using a fixed time step of, if I'm not wrong, 1s. It was not causing any trouble during the first time steps but after a few time steps the Courant number started raising until the end of the simulation leading this to totally unphysical values. When I found it out I started the run with a deltaT of 0.2s during the first second to get it started and afterwards I switched the parameter adjustTimeStep to yes and maxCo to 0.9 in order to get better values for my simulation. Obviously, I got an improved temperature distribution but they are not totally correct yet. Here you can see the result I got, temperature minimums are not as unphysical as they were, but they are not physical at all yet. Thanks for your help and time. Regard, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

May 12, 2015, 13:38 

#28 
Member
Mehtab
Join Date: Jan 2015
Posts: 41
Rep Power: 10 
Hi foamers,
Is there any kind soul to help me solve this problem? I am getting this error while running. I know the problem is coming from boundary condition but I do not know what should I do further. Please help. Code:
#0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 in "/lib64/libc.so.6" #3 Foam::divide(Foam::Field<double>&, double const&, Foam::UList<double> const&) at ??:? #4 Foam::operator/(double const&, Foam::UList<double> const&) at ??:? #5 Foam::customEnthalpyFluxTemperatureFvPatchScalarField::updateCoeffs() at ??:? #6 Foam::mixedFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) at ??:? #7 Foam::mixedEnergyFvPatchScalarField::updateCoeffs() at ??:? #8 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoeffs() at ??:? #9 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at ??:? #10 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:? #11 Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at ??:? #12 Foam::radiation::radiationModel::Sh(Foam::fluidThermo&) const at ??:? #13 at ??:? #14 __libc_start_main in "/lib64/libc.so.6" #15 at /home/abuild/rpmbuild/BUILD/glibc2.19/csu/../sysdeps/x86_64/start.S:125 Floating point exception Thanks in advance.................. 

May 16, 2015, 11:33 

#29 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 127 
Quick answer  Follow the instructions given here: http://www.cfdonline.com/Forums/ope...gethelp.html


January 20, 2016, 01:00 

#30 
Member
laurentL
Join Date: Oct 2011
Location: new caledonia
Posts: 73
Rep Power: 13 
dear all,
i'm still facing a crach of the chtMultiRegionSimpleFoam after 5 time steps here the end of the log file: any suggestion will be very welcome, thank by advance .. Code:
Time = 4 Solving for fluid region air DILUPBiCG: Solving for Ux, Initial residual = 0.1677119, Final residual = 0.007570572, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.09862205, Final residual = 0.005734411, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1516592, Final residual = 0.01006138, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.3224805, Final residual = 0.01444143, No Iterations 2 Min/max T:101.3907 401.5919 GAMG: Solving for p_rgh, Initial residual = 0.4801783, Final residual = 0.004185736, No Iterations 4 time step continuity errors : sum local = 0.2820421, global = 0.01068328, cumulative = 0.02434987 Min/max rho:0.2 2 DILUPBiCG: Solving for epsilon, Initial residual = 0.2375966, Final residual = 0.002033653, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.1964795, Final residual = 0.009602515, No Iterations 2 bounding k, min: 33.28641 max: 1857.522 average: 22.48295 Solving for fluid region fume DILUPBiCG: Solving for Ux, Initial residual = 0.0199697, Final residual = 0.0008280021, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.1334775, Final residual = 0.007614913, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1267019, Final residual = 0.006066752, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.008734778, Final residual = 0.0003510015, No Iterations 2 Min/max T:297.528 873 GAMG: Solving for p_rgh, Initial residual = 0.8375047, Final residual = 0.03764495, No Iterations 1000 time step continuity errors : sum local = 0.6269954, global = 0.01164683, cumulative = 0.0359967 Min/max rho:0.3691154 1.16368 DILUPBiCG: Solving for epsilon, Initial residual = 0.1786266, Final residual = 0.003092718, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.1973878, Final residual = 0.0100348, No Iterations 2 Solving for solid region duct DICPCG: Solving for h, Initial residual = 0.2881169, Final residual = 0.0007063077, No Iterations 1 Min/max T:298.9668 300.4051 ExecutionTime = 10.96 s ClockTime = 11 s Time = 5 Solving for fluid region air DILUPBiCG: Solving for Ux, Initial residual = 0.1466593, Final residual = 0.007074396, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.06904185, Final residual = 0.004619607, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1118558, Final residual = 0.006564061, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.2891947, Final residual = 0.01391482, No Iterations 2 Min/max T:1028.41 1530.922 GAMG: Solving for p_rgh, Initial residual = 0.5476232, Final residual = 0.005112517, No Iterations 8 time step continuity errors : sum local = 0.1420783, global = 0.0001118252, cumulative = 0.03588488 Min/max rho:0.2 2 DILUPBiCG: Solving for epsilon, Initial residual = 0.06832264, Final residual = 0.003890928, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.116786, Final residual = 0.007913494, No Iterations 2 bounding k, min: 19.92499 max: 2166.974 average: 26.66811 Solving for fluid region fume DILUPBiCG: Solving for Ux, Initial residual = 0.06167192, Final residual = 0.002577803, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.2057269, Final residual = 0.01041299, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.2193009, Final residual = 0.01016463, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.005325784, Final residual = 0.0002819179, No Iterations 2 Min/max T:297.252 873 GAMG: Solving for p_rgh, Initial residual = 0.6903963, Final residual = 0.01323959, No Iterations 1000 time step continuity errors : sum local = 0.1716709, global = 0.00316045, cumulative = 0.03272443 Min/max rho:0.2136852 1.341727 DILUPBiCG: Solving for epsilon, Initial residual = 0.06676783, Final residual = 0.001963593, No Iterations 1 DILUPBiCG: Solving for k, Initial residual = 0.1674929, Final residual = 0.007493294, No Iterations 2 Solving for solid region duct DICPCG: Solving for h, Initial residual = 0.4740359, Final residual = 0.0007971916, No Iterations 1 Min/max T:230.8002 335.3638 ExecutionTime = 13.87 s ClockTime = 14 s Time = 6 Solving for fluid region air DILUPBiCG: Solving for Ux, Initial residual = 0.1813033, Final residual = 0.008672431, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.06567908, Final residual = 0.003131843, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.1290634, Final residual = 0.008479523, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.1528493, Final residual = 0.004408951, No Iterations 2 [13] [13] [13] > FOAM FATAL ERROR: [13] Maximum number of iterations exceeded [13] [13] From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>] [13] in file /home/laurent/OpenFOAM/OpenFOAM3.0.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66. [13] FOAM parallel run aborting [13] [13] #0 Foam::error::printStack(Foam::Ostream&) at ??:? [13] #1 Foam::error::abort() at ??:? [13] #2 Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy>::THs(double, double, double) const at ??:? [13] #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:? [13] #4 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:? [13] #5 ? at ??:? [13] #6 __libc_start_main in "/lib64/libc.so.6" [13] #7 ? at /home/abuild/rpmbuild/BUILD/glibc2.19/csu/../sysdeps/x86_64/start.S:125  MPI_ABORT was invoked on rank 13 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them.  

January 20, 2016, 13:59 

#31 
Senior Member

Please revise your boundary conditions.
Also, please check user manual for max number of iterations setting, that you may set unintensionally. Last edited by wyldckat; January 31, 2016 at 11:34. Reason: merged 2 posts that were a few minutes apart from each other 

January 22, 2016, 17:42 

#32 
Member
laurentL
Join Date: Oct 2011
Location: new caledonia
Posts: 73
Rep Power: 13 
hi Ahmed,
thank very much for helping. i post one of the many BC i have try... and a little drawing of the physical problem, gaz going through a pipe. i could not find where to increases the maximum number of iteration... the solution is may be to run a transient solver first? 

January 22, 2016, 18:51 

#34  
Member
laurentL
Join Date: Oct 2011
Location: new caledonia
Posts: 73
Rep Power: 13 
the simulation is running only with laminar option, but the velocity of air goes up to 59 m/s ... for 1m./s at inlet
and if i turn kEpsilon option after 4 times step i got: Quote:


March 28, 2016, 14:22 

#35 
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,969
Blog Entries: 45
Rep Power: 127 
Greetings to all!
I had this thread on my todo list because of laurent98's questions and I finally today managed to take a look into it. Unfortunately, since almost no information was provided about the case setup, I'm not able to even try and guess what's wrong @laurent98: If you have not yet solved this problem in your case, then please follow the instructions given on this thread: http://www.cfdonline.com/Forums/ope...gethelp.html Best regards, Bruno 

March 30, 2016, 12:12 

#36 
Member
Ali
Join Date: Aug 2011
Location: Milwaukee
Posts: 34
Rep Power: 13 
Bruno,
I know this is an old thread but I am facing the exact problem. I'm trying to solve a heat exchanger problem using chtMultiRegionSimpleFoam and the temperature goes to 90 and then it crashes. I opened a new thread a while ago and didnt get any response over there (http://www.cfdonline.com/Forums/ope...implefoam.html) Going through different threads I found out maybe if I run my model as transient for a few time steps and then use that data as my IC it would work. Which it didnt and I am getting the following error: Code:
/**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 3.0.1   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 3.0.1119cac7e8750 Exec : chtMultiRegionFoam Date : Mar 30 2016 Time : 11:07:11 Host : "node1" PID : 31430 Case : /home/cssllab/Desktop/multiRegionHeater nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Allowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region air_domain for time = 0 Create fluid mesh for region water_domain for time = 0 Create solid mesh for region solid_domain for time = 0 *** Reading fluid mesh thermophysical properties for region air_domain Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport polynomial; thermo hPolynomial; equationOfState icoPolynomial; specie specie; energy sensibleEnthalpy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to hRefFluid Adding to ghFluid Adding to ghfFluid Adding to turbulence Selecting turbulence model type RAS Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; C3 0.33; sigmak 1; sigmaEps 1.3; } Radiation model not active: radiationProperties not found Selecting radiationModel none Adding to KFluid Adding to dpdtFluid Adding MRF No MRF models present Adding fvOptions No finite volume options present *** Reading fluid mesh thermophysical properties for region water_domain Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectFluid; specie specie; energy sensibleInternalEnergy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding to hRefFluid Adding to ghFluid Adding to ghfFluid Adding to turbulence Selecting turbulence model type laminar Radiation model not active: radiationProperties not found Selecting radiationModel none Adding to KFluid Adding to dpdtFluid Adding MRF No MRF models present Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region solid_domain Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Radiation model not active: radiationProperties not found Selecting radiationModel none Adding fvOptions No finite volume options present Region: air_domain Courant Number mean: 0.01195979 max: 0.6265122 Region: water_domain Courant Number mean: 0.09387028 max: 0.7258117 Region: solid_domain Diffusion Number mean: 2.409372e05 max: 6.511168e05 Region: air_domain Courant Number mean: 0.01195979 max: 0.6265122 Region: water_domain Courant Number mean: 0.09387028 max: 0.7258117 Region: solid_domain Diffusion Number mean: 2.409372e05 max: 6.511168e05 Time = 0.001 Solving for fluid region air_domain #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::sigFpe::sigHandler(int) at ??:? #2 ? in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #4 Foam::operator/(Foam::UList<double> const&, Foam::UList<double> const&) at ??:? #5 Foam::diagonalSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:? #6 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:? #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:? #8 Foam::fvMatrix<double>::solve() at ??:? #9 ? at ??:? #10 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #11 ? at ??:? Floating point exception (core dumped) (http://www.cfdonline.com/Forums/ope...implefoam.html) Thanks Ali 

March 30, 2016, 15:32 

#37 
Senior Member
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 12 
have you changing the values of the
nNonOrthogonalCorrectors or the relaxationFactors in system/fluid_region/fvSolution? a resource that helped me step up and solve such issues was this http://www.dicat.unige.it/guerrero/o...sandtricks.pdf Cheers, derek Code:
SIMPLE { momentumPredictor on; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 100000; rhoMin rhoMin [1 3 0 0 0] 0.2; rhoMax rhoMax [1 3 0 0 0] 2; } relaxationFactors { fields { rho 1.0; p_rgh 0.7; } equations { U 0.3; h 0.7; "(kepsilonomega)" 0.7; G 0.7; "ILambda.*" 0.7; Qr 0.7; } }
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET 

March 30, 2016, 16:26 

#38 
Member
laurentL
Join Date: Oct 2011
Location: new caledonia
Posts: 73
Rep Power: 13 
Hi Bruno,
thank you very much for your interest, i didn't solve my problem with openfoam yet but i made a simplest computation by hand with classical thermic formulations. please find attach a general presentation of the problem. i'am sorry to not be on my computer now, i have not access right now to my OF's files best regards Laurent 

March 30, 2016, 18:06 

#39 
Member
Ali
Join Date: Aug 2011
Location: Milwaukee
Posts: 34
Rep Power: 13 
Derek,
Thanks for the response. I actually did play with the relaxation factors a lot! My last test was that I fixed the temp. every where to see if the solution still explodes which it did! So, now I'm looking different ways to see if I can find some answers for my problem. 

March 31, 2016, 08:43 

#40 
Senior Member
Alex
Join Date: Oct 2013
Posts: 337
Rep Power: 20 
Hi Laurent!
As per the little information you provided related to your error some posts above, it seems that you are probably using an excessively high time step. Some time ago I faced a very similar problem to yours and setting adjustTimeStep to yes in controlDict helped me a lot! Besides that, check that your inlet and outlet BC's are the proper ones. Hope it helps you a little with your struggle! Best regards, Alex
__________________
Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in! 

Thread Tools  Search this Thread 
Display Modes  

