[amol_patel]

I'm trying to solve a conjugate heat transfer case for a shell and tube heat exchanger, i have created my own geometry of the exchanger and created the mesh and I guess its correct till that point. I m using 4 processors to run a parallel simulation using the chtMultiRegionFoam solver.

I used the "mpirun -np 4 chtMultiRegionFoam -parallel" command to run the simulation.

I m getting this error message as shown below by i have the file in the required location in constant also i copied the polyMesh folder for all the regions in the 0/<region-name>/ folder as well for each region shell, solid and tube.

Create time

Create fluid mesh for region shell for time = 0

--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 1 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.
--------------------------------------------------------------------------
[1]
[1]
[1] --> FOAM FATAL ERROR: (openfoam-2012)
[1] Cannot find file "points" in directory "shell/polyMesh" in times "0" down to constant
[1]
[1]     From virtual Foam::IOobject Foam::fileOperation::findInstance(const Foam::IOobject&, Foam::scalar, const Foam::word&) const
[1]     in file global/fileOperations/fileOperation/fileOperation.C at line 1003.
[1]
FOAM parallel run exiting
[1]
[2]
[2]
[2] --> FOAM FATAL ERROR: (openfoam-2012)
[2] Cannot find file "points" in directory "shell/polyMesh" in times "0" down to constant
[2]
[2]     From virtual Foam::IOobject Foam::fileOperation::findInstance(const Foam::IOobject&, Foam::scalar, const Foam::word&) const
[2]     in file global/fileOperations/fileOperation/fileOperation.C at line 1003.
[2]
FOAM parallel run exiting
[2]
[3]
[3]
[3] --> FOAM FATAL ERROR: (openfoam-2012)
[3] Cannot find file "points" in directory "shell/polyMesh" in times "0" down to constant
[3]
[3]     From virtual Foam::IOobject Foam::fileOperation::findInstance(const Foam::IOobject&, Foam::scalar, const Foam::word&) const
[3]     in file global/fileOperations/fileOperation/fileOperation.C at line 1003.
[3]
FOAM parallel run exiting
[3]
[AMOL:20029] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
[AMOL:20029] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
[AMOL:20029] 2 more processes have sent help message help-mpi-api.txt / mpi-abort

I will add my case file in this link below
https://drive.google.com/drive/folde...Yb?usp=sharing

I don't understand where I'm doing wrong.
I'm doing this project to learn OPENFOAM - any help will be grateful .
Thanks for the help.

[Yann]

Hi,

What OpenFOAM version are you using?
Can you describe your full workflow?

In a multiregion case running in parallel, you should have a polymesh directory containing the region mesh in each processor directory, with a path looking like this : processorX/constant/yourRegionName/polyMesh.

Regards,
Yann

[amol_patel]

Hi,

I am using openFoam-v2012 on windows using the ubuntu 20.04 LTS .

As you said i checked for the polyMesh folder in the location processorX/constant/region_name/ployMesh . but in my case i have processorX/0/region_name/polyMesh.

I guess it might be the issue?? but i don't know exactly.

Thanks,
amol.

[Yann]

Hi Amol,


Yes, this is probably the issue. Can you describe exactly what operations you do on your case, and in which order please?


Regards,
Yann

[amol_patel]

Hi Yann,

I did the following operations
1. creating blockMesh
2. decompose the case in 4 processors using the decomposePar command
3. create a snappyHexMesh in parallel using mpirun -np 4 snappyHexMesh - parallel - overwrite
4. decomposed the regions generated using decomposePar -allRegions command
5. run the solver command mpirun -np 4 chtMultiRegionFoam -parallel

now as i was getting the error then i tried the decomposePar -allRegions -constant command in place of the 4th step . Now i have constant folder in each of the processorX dictionary. now my earlier error got resolved but i m facing a new error.

Entry 'kappaMethod' not found in dictionary "/home/amol/OpenFOAM/amol-v2012/run/trial14/processor2/0/shell/T.boundaryField.shell_to_solid"

so i added the kappaMethod for the shell_to_solid boundary as follows

shell_to_solid
    {
        type        compressible::turbulentTemperatureCoupledBaffleMixed;        
        value           $internalField;
        Tnbr            T;
        kappaMethod     fluidThermo;
    }

again running the solver give me the following error:

Incorrect patch type wall for patch shell_to_solid of field T in file "/home/amol/OpenFOAM/amol-v2012/run/trial14/processor3/0/shell/T"
Type should be a mappedPatch

I dont understand how it should be a mappedPatch and if i change the type of shell_to_solid from compressible::turbulentTemperatureCoupledBaffleMix ed to mappedPatch is shows that i have used the wrong patch name and the list of patchnames doesnt include mappedPatch.

please help me .

Thanks,
amol.

[Yann]

Hi Amol,

The 4th step is wrong. After running snappyHexMesh in parallel, the mesh is already decomposed in each processor directory. But you need to use the splitMeshRegions utility to split your whole mesh in separate meshes for each region. Usually this is the command we use:

mpirun -np 4 splitMeshRegions -cellZones -overwrite -parallel

Then you can run your solver as stated in the 5th step of your post.

I think this should solve your mappedPatch problem.

Let us know how it goes,
Yann

[amol_patel]

i m so sorry to mention that step i had already used that command to split the mesh regions.

i m really sorry for not adding that step while writing the steps earlier.

Thanks,
amol.

[Yann]

OK then it should be fine, but still you don't have to run the decomposePar -allRegions written at the 4th step of your previous post.
Does it run properly now?

All the commands you run are important, and the order in which you run it is important too.

Yann

[amol_patel]

Hi Yann,

A quick update so now i guess i have made all the small corrections that were generated during the solver running step.
now the solver starts but as recongnizes the case but now it stops giving the following error:

WARNING: Linux kernel CMA support was requested via the
btl_vader_single_copy_mechanism MCA variable, but CMA support is
not available due to restrictive ptrace settings.

The vader shared memory BTL will fall back on another single-copy
mechanism if one is available. This may result in lower performance.

  Local host: AMOL
--------------------------------------------------------------------------
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2012                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : _7bdb509494-20201222 OPENFOAM=2012
Arch   : "LSB;label=32;scalar=64"
Exec   : chtMultiRegionFoam -parallel
Date   : Oct 14 2021
Time   : 11:42:40
Host   : AMOL
PID    : 648
I/O    : uncollated
Case   : /home/amol/OpenFOAM/amol-v2012/run/trial14
nProcs : 4
Hosts  :
(
    (AMOL 4)
)
Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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

Create fluid mesh for region shell for time = 0

Create fluid mesh for region tube for time = 0

Create solid mesh for region solid for time = 0

*** Reading fluid mesh thermophysical properties for region shell

    Adding to thermoFluid

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to hRefFluid

    Adding to ghFluid

    Adding to ghfFluid

    Adding to turbulenceFluid

Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
    model           kEpsilon;
    turbulence      on;
    printCoeffs     on;
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              0;
    sigmak          1;
    sigmaEps        1.3;
}

    Adding to reactionFluid

Combustion model not active: combustionProperties not found
Selecting combustion model none
    Adding to radiationFluid

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid

    Adding to fieldsFluid

    Adding to QdotFluid

    Adding MRF

No MRF models present

    Adding fvOptions

*** Reading fluid mesh thermophysical properties for region tube

    Adding to thermoFluid

Selecting thermodynamics package
{
    type            heRhoThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState rhoConst;
    specie          specie;
    energy          sensibleEnthalpy;
}

[AMOL:00644] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied
[AMOL:00644] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages
    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to hRefFluid

    Adding to ghFluid

    Adding to ghfFluid

    Adding to turbulenceFluid

Selecting turbulence model type RAS
Selecting RAS turbulence model kEpsilon
RAS
{
    model           kEpsilon;
    turbulence      on;
    printCoeffs     on;
    Cmu             0.09;
    C1              1.44;
    C2              1.92;
    C3              0;
    sigmak          1;
    sigmaEps        1.3;
}

    Adding to reactionFluid

Combustion model not active: combustionProperties not found
Selecting combustion model none
    Adding to radiationFluid

Radiation model not active: radiationProperties not found
Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid

    Adding to fieldsFluid

    Adding to QdotFluid

    Adding MRF

No MRF models present

    Adding fvOptions

*** Reading solid mesh thermophysical properties for region solid

    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

Region: shell Courant Number mean: 0 max: 0
Region: tube Courant Number mean: 0 max: 0
Region: solid Diffusion Number mean: 196.871 max: 28764.9
Region: shell Courant Number mean: 0 max: 0
Region: tube Courant Number mean: 0 max: 0
Region: solid Diffusion Number mean: 196.871 max: 28764.9
Time = 1


Solving for fluid region shell
--------------------------------------------------------------------------
Primary job  terminated normally, but 1 process returned
a non-zero exit code. Per user-direction, the job has been aborted.
--------------------------------------------------------------------------
--------------------------------------------------------------------------
mpirun detected that one or more processes exited with non-zero status, thus causing
the job to be terminated. The first process to do so was:

  Process name: [[64410,1],0]
  Exit code:    144
--------------------------------------------------------------------------

So now I'm stuck again.
Is it because the solid diffusion number is high ? or the fluid courant number being 0 ?
But as is reduce the timestep value from 1 to 0.01 the diffusion number decreases but the courant number is 0.


Thanks,
amol.

[Yann]

It can be related to a lot of things, this is hard to say without knowing more about your case setup. First guess would be to check the boundary conditions and initialization, but the problem might lie somewhere else too.

Relatively to your Courant and Diffusion numbers, you can try starting with a smaller time step and use the adjustTimeStep function in controlDict. Here is the one from the snappyMultiRegionHeater tutorial:

maxCo           0.3;
maxDi           10.0;
adjustTimeStep  yes;

The solver crashes when solving the fluid region "shell" so you should start looking there first.

Yann

[amol_patel]

Hi Yann,

Sorry for the late reply i was all caught up,
I have been trying to find the solution for the but was unsuccessful.
Although I was able to get the courants numbers calculated but the solver stops at the same point that is after calculating the courant numbers and the diffusion number.

I m uploading my case file here. Can you please check my files and point out what is wrong .

I have kept the following files whiles sharing due to size factors

0
>>shell
>>>>alphat,U,T,p,p_rgh,k,epsilon,nut,rho,cellToReg ion
>>tube
>>>>alphat,U,T,p,p_rgh,k,epsilon,nut,rho,cellToReg ion
>>solid
>>>>cellToRegion,T,p

constant
>>(ployMesh>boundary),g,regionproperties
>>shell
>>>>(ployMesh>boundary),g,thermophysicalProperties ,transportProperties
>>tube
>>>>(ployMesh>boundary),g,thermophysicalProperties ,transportProperties
>>solid
>>>>(ployMesh>boundary),thermophysicalProperties

system
>>blockMeshDict,controlDict,snappyHexMeshDict,deco mposeParDict,fvSchemes,fvSolution,residuals
>>shell
>>>>decomposeParDict,fvSchemes,fvSolution
>>tube
>>>>decomposeParDict,fvSchemes,fvSolution
>>solid
>>>>decomposeParDict,fvSchemes,fvSolution

ThankYou,
amol

[Yann]

Hi Amol,

Without the geometry I cannot run your case
After having a look at it, it seems strangely similar to the shellAndTubeHeatExchanger tutorial from the OpenFOAM foundation branch.

Is it the case you used to start setting up your case?
If yes, have you tried running the original tutorial with OpenFOAM-v2012 before starting to modify it?

Yann

[amol_patel]

Hi Yann,

As you said it is true first is did run a tutorial case and at that time it ran well but there is used openfoam-8 on virtual box .

I then shifted to WSL (ubuntu 20.04 ) as i have bigger geometry and virtual box was not running smoothly.

In the WSL i downloaded openfoam-v2012 as i was unaware that version change may have any affect.

Now, when i used my geometry to run the case i get this error.

sorry that i cant upload my geometry as it goes beyond the size for this forum.

Regards,
amol.

[Yann]

The ESI-OpenCFD branch (openfoam.com) and OpenFOAM foundation branch (openfoam.org) are different despite their common origin. If you take a case from one version, you will often have to adapt it to be able to run the case on another version.

On WSL you can use both branches so I would suggest you to install OpenFOAM-8, run the shellAndTubeHeatExchanger tutorial and then work from there to adapt the case to your own geometry.

If you still want to use OpenFOAM-v2012, try running the original shellAndTubeHeatExchanger tutorial from OpenFOAM-8 on v2012 first to see if it works on v2012 before trying to modify the case with your own geometry.

Regards,
Yann

[amol_patel]

Thanks alot Yann for giving me all the advice.

I will try to follow the step as you say and i will get back to you.

Thanks
amol

[amol_patel]

Hi Yann,

I changed to openfoam-8 and first tried the tutorial .
Now i created the mesh for my case now I m getting this error while running the chtMultiRegionFoam solver

Solving for fluid region shell
DILUPBiCGStab:  Solving for Ux, Initial residual = 1, Final residual = 9.98003e-08, No Iterations 89
DILUPBiCGStab:  Solving for Uy, Initial residual = 1, Final residual = 7.00312e-08, No Iterations 91
DILUPBiCGStab:  Solving for Uz, Initial residual = 1, Final residual = 9.9678e-08, No Iterations 143
DILUPBiCGStab:  Solving for h, Initial residual = 1, Final residual = 8.04366e-08, No Iterations 60
Min/max T:299.997 1.43204e+06
 --> FOAM FATAL ERROR:
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 1081.1
Specified mass inflow   : 0.5
Specified mass outflow  : 0
Adjustable mass outflow : 1.58279e-15

I tired changing the velocity and pressure files
also i dont understand my temperature ranges are 300 and 600 so how the max temperature increases to so high value.

U File =>

FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0/shell";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [ 0 1 -1 0 0 0 0 ];

internalField uniform (0 0 0);

boundaryField
{

shell_inlet
{
type flowRateInletVelocity;
massFlowRate constant 0.5;
rho rho;
rhoInlet 1000;
}
shell_outlet
{
type pressureInletOutletVelocity;
value $internalField;
}
solid_solid
{
type noSlip;
}
shell_walls
{
type noSlip;
}
shell_to_solid
{
type noSlip;
}
}


p file =>

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0/shell";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [ 1 -1 -2 0 0 0 0 ];

internalField uniform 0;

boundaryField
{

shell_inlet
{
type calculated;
value $internalField;
}
shell_outlet
{
type calculated;
value $internalField;
}
shell_walls
{
type calculated;
value $internalField;
}
shell_to_solid
{
type calculated;
value $internalField;
}
solid_solid
{
type calculated;
value $internalField;
}
}


T file =>
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0/shell";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [ 0 0 0 1 0 0 0 ];

internalField uniform 600;

boundaryField
{

shell_inlet
{
type fixedValue;
value uniform 600;
}
shell_outlet
{
type zeroGradient;
//value uniform 600;
//inletValue uniform 600;
}
shell_walls
{
type zeroGradient;
}
solid_solid
{
type zeroGradient;
}
shell_to_solid
{
type compressible::turbulentTemperatureCoupledBaffleMix ed;
value uniform 600;
Tnbr T;
kappaMethod fluidThermo;
}
}


also p_rgh file =>

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0/shell";
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [ 1 -1 -2 0 0 0 0 ];

internalField uniform 0;

boundaryField
{

shell_inlet
{
type fixedFluxPressure;
value $internalField;
}
shell_outlet
{
type fixedValue;
value $internalField;
}
shell_walls
{
type fixedFluxPressure;
value $internalField;
}
shell_to_solid
{
type fixedFluxPressure;
value $internalField;
}
solid_solid
{
type fixedFluxPressure;
value $internalField;
}
}


Can you please suggest me what is going wrong here.

Thanks,
amol

[Yann]

Hi Amol,

Something is wrong with your Boundary Conditions.

In processor*/constant/shell/polyMesh/boundary, check what boundary types you have. It should be type patch on the inlet an outlet.

If this is not the case, you can update the boundary file to set "type patch" on your inlet/outlet patches using the changeDictionary utility.

If inlet/outlet are already set to "type patch", please upload your case and I'll have a look.

Yann

[amol_patel]

Hi Yann,

I have been working on this and have made a lot of changes finally the simulation runs.

But we have a situation
1. the adjust timestep feature make jumps of the order of e-5 seconds which make it very slow
2. the velocity at the outlet for the shell and tube is very high

I am adding my case here , I have added the stl files for the required in the form of zip files.
Please can you check my case.

Thanks,
amol

[Yann]

Hi Amol,


Can you provide a script with your case in order to reproduce all the steps you are doing to mesh and run your case?



Yann

[amol_patel]

Hi Yann,

I am using the following steps to run my case:

1. blockMesh
2. snappyHexMesh -overwrite
3. splitMeshRegions -cellZonesOnly -constant
4. decomposePar
5. decomposePar -allRegions
6. mpirun -np 4 chtMultiRegionFoam -parallel

I ran the case for sometime so that we get few timesteps stored.
After that I see the results in paraview.