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

buoyantBoussinesqSimpleFoam: Floating point exception (core dumped)

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 26, 2014, 18:01
Default buoyantBoussinesqSimpleFoam: Floating point exception (core dumped)
  #1
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
I'm trying to model a solar chimney based on Boussinesq model. After a few time steps I get this error:

Code:
Time = 13

DILUPBiCG:  Solving for Ux, Initial residual = 9.40767e-05, Final residual = 9.32478e-07, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.000374868, Final residual = 7.71871e-06, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.00110305, Final residual = 2.33651e-05, No Iterations 1
DILUPBiCG:  Solving for T, Initial residual = 0.0675763, Final residual = 0.000322582, No Iterations 1
#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::DICPreconditioner::calcReciprocalD(Foam::Field<double>&, Foam::lduMatrix const&) at ??:?
#4  Foam::DICPreconditioner::DICPreconditioner(Foam::lduMatrix::solver const&, Foam::dictionary const&) at ??:?
#5  Foam::lduMatrix::preconditioner::addsymMatrixConstructorToTable<Foam::DICPreconditioner>::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) at ??:?
#6  Foam::lduMatrix::preconditioner::New(Foam::lduMatrix::solver const&, Foam::dictionary const&) at ??:?
#7  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#8  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
#9  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#10  
 at ??:?
#11  
 at ??:?
#12  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#13  
 at ??:?
Floating point exception (core dumped)
This is my checkMesh:

Code:
Build  : 2.3.0-f5222ca19ce6
Exec   : checkMesh
Date   : Oct 26 2014
Time   : 18:57:25
Host   : "raghav"
PID    : 5903
Case   : /home/raghav/OpenFOAM/raghav-2.3.0/run/solarChimney
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           1449
    internal points:  0
    faces:            9305
    internal faces:   6411
    cells:            3929
    faces per cell:   4
    boundary patches: 5
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    3929
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    blackWall           1250     692      ok (non-closed singly connected)  
    glassWall           1328     731      ok (non-closed singly connected)  
    outlet              67       64       ok (non-closed singly connected)  
    inlet               75       69       ok (non-closed singly connected)  
    wall                174      173      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (4.2 4 6)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (1.67772e-16 -9.04982e-17 -9.41181e-19) OK.
    Max cell openness = 2.08637e-16 OK.
    Max aspect ratio = 5.98181 OK.
    Minimum face area = 0.00145422. Maximum face area = 0.129964.  Face area magnitudes OK.
    Min volume = 3.4493e-05. Max volume = 0.00620352.  Total volume = 4.8.  Cell volumes OK.
    Mesh non-orthogonality Max: 62.114 average: 21.9416
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.583302 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End
I think the mesh is okay. When I see the solution, the velocities are very high, indicating the solution has diverged. Does anyone know what the error means and where the problem is? Case attached.

Thanks
Attached Files
File Type: gz solarChimney.tar.gz (94.3 KB, 21 views)
raghav.venky is offline   Reply With Quote

Old   October 27, 2014, 03:28
Default
  #2
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,938
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

Could you describe the case in more details? From your case files:

1. Boundaries walls, glassWall, and blackWall overlap. Not quite sure it's good decision to have them this way.
2. Thickness of the mesh is 1 cell, are you quite sure this is what you want? And this cell is in direction of temperature gradient.
3. Mesh is tetrahedral, use leastSquares for gradient schemes.
4. You'd like to use k-epsilon turbulence model, are you sure your case is turbulent?
alexeym is offline   Reply With Quote

Old   October 27, 2014, 09:26
Default
  #3
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
@alexeym

Thanks for your input.

1. I don't understand what you mean by that. The three surfaces are distinct and are either parallel or perpendicular to each other. Can you please what you mean by overlap?

2. Yes I thought that was not good. I used Salome to generate the mesh. I don't know how to refine the mesh in one direction and keep it coarse in the other directions. I'll make the entire mesh fine and then see what happens.

3. I did not know this. Is there a place where I can read up on this?

4. I thought buoyantBoussinesqSimpleFoam has to be turbulent. Is there a way to turn it off? I'll simulate non turbulence and then go on to turbulence.


I'll post the results after I make the changes you've suggested in a few days.

Thanks!
raghav.venky is offline   Reply With Quote

Old   October 27, 2014, 09:52
Default
  #4
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,938
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
Hi,

1. It seems, this was my mistake, paraview messed up wall as patch name and wall as a group of patches, so it displayed wall patch as group of patches (wall + backWall + glassWall), that's why I thought they overlap.

2. The geometry of the mesh is very simple, I don't know why you'd like to use Salome instead of blockMesh.

3. http://www.cfd-online.com/Forums/ope...mesh-pipe.html, https://www.google.fr/search?q=openf...s+grad+schemes

4. There's turbulence model called "laminar", if you take a look at the code

Code:
tmp<volScalarField> laminar::nut() const
{
    return tmp<volScalarField>
    (
        new volScalarField
        (
            IOobject
            (
                "nut",
                runTime_.timeName(),
                mesh_,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            mesh_,
            dimensionedScalar("nut", nu()().dimensions(), 0.0)
        )
    );
}
so nuEff == nu + nut is just nu, i.e. molecular viscosity.
alexeym is offline   Reply With Quote

Old   October 28, 2014, 19:31
Default
  #5
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
Used blockMesh to generate mesh. Hence not using leastSquares for gradient schemes. Looks like there is no option (ie turbulenceProperties dictionary) to make it laminar for buoyantBoussinesqSimpleFoam. I tried turning off turbulence in the RASProperties (in the constant directory). The solution still diverges. I've attached the case files.

Could the boundary conditions be a problem?
Attached Files
File Type: gz solarChimney.tar.gz (19.5 KB, 16 views)
raghav.venky is offline   Reply With Quote

Old   October 28, 2014, 19:58
Default
  #6
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
I played around. Set the velocity boundary condition at the inlet and outlet as 0. Now no air can come in or go out. I get a nice circulation of the air inside ie the air near the hot boundary rises and the air near cold boundary falls.

Now, to simulate air entering and and leaving ie driven due to buoyancy, I had given a zeroGradient boundary condition. But this led divergent solutions. Any suggestions?
raghav.venky is offline   Reply With Quote

Old   October 29, 2014, 03:48
Default
  #7
Senior Member
 
Alexey Matveichev
Join Date: Aug 2011
Location: Nancy, France
Posts: 1,938
Rep Power: 38
alexeym has a spectacular aura aboutalexeym has a spectacular aura about
Send a message via Skype™ to alexeym
You can try starting with transient solver instead of steady state. Also you can increase under-relaxation, though it led to inconsistency between inlet and outlet (i.e. amount of mater added to the system wasn't equal to amount of removed matter) with zeroGradient BCs.
alexeym is offline   Reply With Quote

Old   November 4, 2014, 10:58
Default
  #8
Member
 
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 13
hanness is on a distinguished road
Hi Raghav,

you could try with a fixedValue pressure on the inlet and a zeroGradient on the outlet or vice versa which would be a common setup for flows through a domain. Usually you would provide the velocity accordingly (fixedValue for velocity where pressure is zeroGradient and vice versa)
For open boundaries you could also try a totalPressure boundary condition for p_rgh and inletOutlet or pressureInletOutletVelocity for U.
For buoyancy driven flows exposed to the ambient I usually use a modified totalPressure BC for p_rgh on both inlet and outlet (modified to account for the barometric pressure differences) and pressureInletOutletVelocity for U. That works fine for large scale simulations.

Hopefully one of those combinations works for you.
Hannes
hanness is offline   Reply With Quote

Old   November 8, 2014, 22:22
Default
  #9
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
@alexeym and @hanness

Thank you very much for your suggestions. Sorry for the delayed response, I've been busy with other stuff. The closed system (0 velocity inlet and outlet) is very interesting and I'll be working on that for a while. Is there way to get the heat transfer rate or the heat transfer coefficient?

I believe it starts with getting the gradient of the temperature on the surface where I want to find the heat transfer. Is there a way to do that?

Also, I will have to get the heat flux or the heat transfer coefficient. I have no idea how to do that.
raghav.venky is offline   Reply With Quote

Old   November 19, 2014, 05:15
Default
  #10
Member
 
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 13
hanness is on a distinguished road
Hi Raghav,

have a look at the wallHeatFlux utility coming with OpenFOAM.

Hannes
hanness is offline   Reply With Quote

Old   November 22, 2014, 12:29
Default
  #11
New Member
 
Raghav
Join Date: Oct 2014
Posts: 12
Rep Power: 11
raghav.venky is on a distinguished road
Thanks hanness, that was helpful
raghav.venky is offline   Reply With Quote

Old   June 30, 2019, 13:33
Default
  #12
New Member
 
Mateo
Join Date: Jun 2019
Posts: 3
Rep Power: 6
mathew1105 is on a distinguished road
hi sorry , how do you calculate the Totalpressure at the outlet and inlet for a buoyancy flow?

I am stock with a similar problem and am facing convergene problems


thank you for your help
mathew1105 is offline   Reply With Quote

Reply

Tags
boussinesq, core dumped, solar chimney

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
Floating Point Exception Error nyox FLUENT 11 November 30, 2018 12:31
Inlet Velocity Profile BC - Floating Point exception during solution initialization Janshi STAR-CCM+ 4 March 14, 2012 10:21
simpleFoam Floating point exception error -help sudhasran OpenFOAM Running, Solving & CFD 3 March 12, 2012 16:23
Pipe flow in settlingFoam floating point exception jochemvandenbosch OpenFOAM Running, Solving & CFD 4 February 16, 2012 03:24
block-structured mesh for t-junction Robert@cfd ANSYS Meshing & Geometry 20 November 11, 2011 04:59


All times are GMT -4. The time now is 18:21.