[zfaraday]

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:

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/glibc-2.17/csu/../sysdeps/x86_64/start.S:126

Althoug it's not exactly the same message that appeared to the thread's creator (mine seems to be related to some BC, but I don't know exactly which one nor what the problem is...) I followed the steps that Bruno Santos suggested. I check the mesh topology and I found that

    Cell determinant (wellposedness) : minimum: 0 average: 3.2312708
 ***Cells with small determinant (< 0.001) found, number of cells: 960
  <<Writing 960 under-determined cells to set underdeterminedCells

Seeing this error I understood that I had exactly the same problem than the creator of the thread, although the message was not exctly the same... Well, first of all I would really like to know what exactly means this error and what an under determined cell is, because the under determined cells in my case belong to some thin regions that are made up of only one column of cells. I actually solved this error by dividing these regions into more columns of cells in the blockMeshDict file.

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

[wyldckat]

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:

1. You're using groovyBC. Not that it's dangerous by itself, the problem is that apparently you're not experienced enough with it. Therefore, the first step would be for you to first put aside using groovyBC for now, until you can figure out what is the reason for the problem.
2. You're trying to use variables that are defined only at the end of the file "T". I'm not even sure what to say here... mmm, I guess that this is a good analogy: I'll tell you why this is a problem, after you've spent some time reading a least one good C++ book

Best regards,
Bruno

[zfaraday]

Dear Bruno,

Thanks for your quick answer!

Originally Posted by wyldckat

Greetings Alex,

In a case like this, you should apply the good old strategy of "isolate and conquer".

The wiser advise you could ever give in a case like mine. However, as I am trying to be as wise as you, I already isolated but I'm still waiting for my conquest to come...

Originally Posted by wyldckat

Anyway, from what I can see in the "T" file you provided, there are two major threats:

1. You're using groovyBC. Not that it's dangerous by itself, the problem is that apparently you're not experienced enough with it. Therefore, the first step would be for you to first put aside using groovyBC for now, until you can figure out what is the reason for the problem.

1. As I mentioned in other posts and you noticed somehow, I'm not an experienced swak user. Nevertheless, finally yesterday I could manage to solve the problem with groovyBC. The problem was that the boundary of the solid region needed a variable coming from a function object I forgot to define in controlDict. I defined it for the fluid region but forgot to do so for the solid region. Thus, I managed to solve my problem!
   
   

   Originally Posted by wyldckat

   You're trying to use variables that are defined only at the end of the file "T". I'm not even sure what to say here... mmm, I guess that this is a good analogy: I'll tell you why this is a problem, after you've spent some time reading a least one good C++ book

That sentence reminds me of something... Maybe some advice I gave to a novice recently... Are you attacking me with my own weapons? Well, you are right, my C++ skills are more than weak, but I found no time to learn something about it on my own so far. However, I know something about C language and I know that declaration of variables goes at the top of the file, not at the bottom. I guess that something like that happens in C++... By the way, I didn't put the variable definition at the bottom, the fact that they are in there is because of what we talked about a couple of days ago.

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):

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 = 3.1317423e-08, No Iterations 7
DILUPBiCG:  Solving for Uy, Initial residual = 0.30021911, Final residual = 6.5293486e-09, No Iterations 8
DILUPBiCG:  Solving for Uz, Initial residual = 0.06714822, Final residual = 1.6341749e-08, No Iterations 7
DILUPBiCG:  Solving for h, Initial residual = 0.060831265, Final residual = 1.0189158e-08, 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 = 9.9287594e-08, No Iterations 10
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (cambra_aire): sum local = 1.3786288e-06, global = -3.2030593e-07, 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 = 2.3456257e-08, No Iterations 8
DILUPBiCG:  Solving for Uy, Initial residual = 0.56513797, Final residual = 5.357496e-08, No Iterations 8
DILUPBiCG:  Solving for Uz, Initial residual = 0.29594071, Final residual = 1.6331144e-08, No Iterations 8
DILUPBiCG:  Solving for h, Initial residual = 0.35403101, Final residual = 1.7882418e-08, 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 = 9.248029e-08, No Iterations 20
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (cambra_aire): sum local = 2.9077841e-06, global = 7.1199841e-08, 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 = 1.1467818e-08, No Iterations 11
DILUPBiCG:  Solving for Uy, Initial residual = 0.7633537, Final residual = 2.8147703e-08, No Iterations 12
DILUPBiCG:  Solving for Uz, Initial residual = 0.73226472, Final residual = 2.7058083e-08, No Iterations 11
DILUPBiCG:  Solving for h, Initial residual = 0.96491629, Final residual = 8.0298622e-09, 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/OpenFOAM-2.3.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/glibc-2.17/csu/../sysdeps/x86_64/start.S:126

The problem comes from the inlet patch where the T falls bellow 0 and its value is going down for the last steps. This problem is only coming from one or maybe two cells whose faces belong to the patch, its velocity is raising very fast and its temperature falls. I attach the velocity, temperature and pressure definition at both patches (inlet&outlet)

• T:
  

      up //outlet
      {
          type            inletOutlet;
          value           uniform 311.15;
          inletValue      uniform 311.15;
      }
      down //inlet
      {
          type            fixedValue;
          value           uniform 311.15;
      }

• P_rgh:
  

      up
      {
          type            fixedValue;
          value           uniform 100000;
      }
      down
      {
          type            fixedValue;
          value           uniform 100000;
      }

• U:
  

      up
      {
          type            pressureInletOutletVelocity;
          value           uniform ( 0 0 0.001 );
          phi             phi;
          rho             rho;
          tangentialVelocity uniform ( 0 0 0 );
      }
      down
      {
          type            pressureInletOutletVelocity;
          value           uniform ( 0 0 0.001 );
          phi             phi;
          rho             rho;
          tangentialVelocity uniform ( 0 0 0 );

  }

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

[wyldckat]

Hi Alex,

temperatures below 0 Kelvin...
It's very much possible that you're triggering an issue related to simulating heat transfer with a steady-state solver. This was addressed sometime ago in another thread... ah, here you go, start reading from here: http://www.cfd-online.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

[zfaraday]

Hi Bruno,

Thanks for the link but it's not exactly the same problem since my case is a transient one, not steady-state. 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

[derekm]

Originally Posted by zfaraday

Hi Bruno,

Thanks for the link but it's not exactly the same problem since my case is a transient one, not steady-state. ...

Alex

thread title is chtmultiregionsimplefoamwhich suggests steadystate.
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.

[zfaraday]

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

[mehtab]

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.

#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/glibc-2.19/csu/../sysdeps/x86_64/start.S:125
Floating point exception

Thanks in advance..................

[wyldckat]

Originally Posted by firefoam

Is there any kind soul to help me solve this problem?

Quick answer - Follow the instructions given here: http://www.cfd-online.com/Forums/ope...-get-help.html

[laurent98]

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 ..

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/OpenFOAM-3.0.1/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/glibc-2.19/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.
--------------------------------------------------------------------------

[Ahmed Khattab]

Please revise your boundary conditions.

Also, please check user manual for max number of iterations setting, that you may set unintensionally.

[laurent98]

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?

[Ahmed Khattab]

Hi Laurant,

I think you have a problem with your air velocity and pressure boundary conditions. Try converting inlet pressure and outlet velocity to zero gradient

[laurent98]

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:

Time = 4


Solving for fluid region air
DILUPBiCG: Solving for Ux, Initial residual = 0.322841, Final residual = 0.01321862, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.7966811, Final residual = 0.01263297, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.5848599, Final residual = 0.01065549, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.9923653, Final residual = 0.02202294, No Iterations 2
Min/max T:-61693.21 78219.37

thank you for helping

[wyldckat]

Greetings to all!

I had this thread on my to-do 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 set-up, 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.cfd-online.com/Forums/ope...-get-help.html

Best regards,
Bruno

[alib022]

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.cfd-online.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:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 3.0.1-119cac7e8750
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 run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied 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: 2.409372e-05 max: 6.511168e-05
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: 2.409372e-05 max: 6.511168e-05
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_64-linux-gnu/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_64-linux-gnu/libc.so.6"
#11  ? at ??:?
Floating point exception (core dumped)

I was wondering if you can take a look at my thread and let me know what am I doing wrong.
(http://www.cfd-online.com/Forums/ope...implefoam.html)

Thanks
Ali

[derekm]

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

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;
        "(k|epsilon|omega)" 0.7;
        G               0.7;
        "ILambda.*"     0.7;
        Qr              0.7;
    }
}

[laurent98]

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

[alib022]

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.

[zfaraday]

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