Hello

[Mukut]

Hello all,

Can I post in English to get support about openFoam?

Thank you

[ohbuchi]

Hi, Mukut,

Yes, of course you can do it!
But I recommend that before it you should post to OpenFOAM-Forum in CFD-Online.
http://www.cfd-online.com/Forums/openfoam/

M.Obuchi,

2013年10月9日水曜日 14時20分52秒 UTC+9 Mukut:

[Mukut]

Thank you Mr. M.Obuchi,

I already posted my problem there...

I got one reply and try to follow his instruction but still there is problem.

Best regards,
MuKuT

[ohbuchi]

Hi, MuKuT,

I've seen your post in OpenFoam-Forum.
Okay, please tell us your problems in detail.
If your OpenFoam outputs error messages, please show these messages too.


2013年10月9日水曜日 15時20分54秒 UTC+9 Mukut:

[Mukut]

Thanks for your co-operation Mr. M. Ohbuchi 

I have modified the domain from the tutorial "multi region heater" of chtMultiRegionFoam. My flow domain is like attached image [a].

In the original tutorial (multi region heater) regions were named as topAir, bottomAir, heater (in my case as dielectric), leftSolid (in my case top electrode), rightSolid (in my case bottom electrode) , I only added another region called innerElec for embedded electrode. In paraFoam when I activate "include zone", all above mentioned regions have been shown in left side panel of paraFoam but why there is no folder created in system folder for innerElec? Rather I found three folders named as domain2, domain3, domain4, each of them have blank fvSchemeDict and fvSolutionDict file..... Have a look in attached image of system folder [image b]

What is the problem?

Thanks

Best regard
Mukut

[ohbuchi]

How did you make your mesh?

In that tutorial, base mesh was made using blockMesh utility in single domain.

Then topoSet utility was used to make cell zones corresponds to each region.
Finally the mesh was split into several regions with splitMeshRegions utility.

So I think your topoSetDict is not included your correct region's name.

Please check it.

2013年10月9日水曜日 16時18分58秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

The base mesh was made using blockmesh, in the previous attached image (a), I only show the regions those were made using toposetDict. But when I execute following command in terminal

splitMeshRegions -cellZones -overwrite

following error has been shown in terminal:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : splitMeshRegions -cellZones -overwrite
Date   : Oct 08 2013
Time   : 15:23:24
Host   : "mukut-Endeavor-MR3300"
PID    : 5370
Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0

Creating single patch per inter-region interface.



--> FOAM FATAL ERROR: 
Cell 19864 with cell centre (0.00225 -2.3312467e-05 -0.009) is multiple zones. This is not allowed.
It is in zone innerelec and in zone bottomAir

    From function getZoneID(..)
    in file splitMeshRegions.C at line 1208.

FOAM exiting 

Thank you

[Mukut]

Dear Ohbuchi san,

Actually I am a new user of openFoam. I am using openfoam since August 2013. May be I made a silly mistake. I am confused about the line

Cell 19864 with cell centre (0.00225 -2.3312467e-05 -0.009) is multiple zones. This is not allowed.
It is in zone innerelec and in zone bottomAir

But the region innerElect which is a inner electrode and is inside of heater (I didn't change the name, used it as a dielectric material) but error message showed that cell 19864 is in a zone innerelec and bottom air. I think if splitMeshRegion works properly, then folder for innerelec will created.

Thanking you

[ohbuchi]

The problem is your topoSetDict.

The cell 19864 is contained in two regions, innerelec and bottomAir.

Then cellZones were defined incompletely in your polyMesh directory,

undefined region's name was automatically named like "domain1".

Please check your topoSetDict about the definition cellZone for these regions.


2013年10月9日水曜日 19時27分40秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

Ohaiyo Guzaimashu

I also think that the problem is in the topoSetDict.
In my domain, innerelec is inside of heater (which is dielectric in my case) not inside bottom air... 
Besides, in the tutorial of Multi Region Heater is like as follows:


Here in middle there is T shape heater and bottom air is defined as "bottomAir is all the other cells"...

but in my case, bottomAir is not with all the other cells, like inner electrode is inside of dielectric and no contact with bottom air.....

I think there is some problems in topoSetDic for my case. If I define bottomAir region like topAir, not bottomAir is with all the other cells...does it work?

best regards,

Mukut

[ohbuchi]

Good morning, Mukut

Please attach your topoSetDict and blockMeshDict with rough drawing of your computational domain.
I will check for you.

The region of "innerelec" is inside the region "dielectric", so the topoSetDict for these regions would be
as follows;

// innerelec
{                                               // make cellSet for innerelec
    name innerelec;
    type cellSet;
    action new;
    source boxToCell;
    sourceInfo { box (x1 y1 z1)(x2 y2 z2) }    // bounding box for innerelec region
}
{                                               // make cellZone from cellSet "innerelec"
  name innerelec;
  type cellZoneSet;
  action new;
  source setToCellZone;
  sourceInfo { set innterelec };          
}

//  dielectric
{                                   // make cellSet for dielectric include innerelec
  name dielectric;
  type cellSet;
  action new;
  source boxToCell;
  sourceInfo { box( (x3 y3 z3)(x4 y4 z4) }              // bouding box for dielectric region 
}
{                                               // remove innerelec from dielectric cellSet
   name dielectric;
   type cellSet;
   action delete;
   source cellToCell;
   sourceInfo { set innerelec };
}
{                                              // make cellZone from cellSet "dielectric"
  name dielectric;
  type cellZoneSet;
  action new;
  source setToCellZone;
  sourceInfo { set dielectric };

}

If the shape of each region is more complex, more set operation would be needed.


M.Ohbuchi

[ohbuchi]

Hi, Mukut,

In your definition for "bottomAir", there isn't contribution of innerelec on cellSet before "action invert".
Therefore, obtained "bottomAir" region includes "innerelec" region.

Please modify your topoSetDict as follows;

     {
        name    bottomAir;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set topAir;
        }
    }
    {                                          <- insert this lines
        name    bottomAir;            <- insert this lines
        type    cellSet;                  <- insert this lines
        action  add;                      <- insert this lines
        source  cellToCell;            <- insert this lines
        sourceInfo                        <- insert this lines
        {                                      <- insert this lines
            set innerelec;               <- insert this lines
        }                                      <- insert this lines
    }                                          <- insert this lines
    {
        name    bottomAir;
        type    cellSet;
        action  invert;
    }
    {
        name    bottomAir;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set bottomAir;
        }
    }
);

// ************************************************************************* //


2013年10月10日木曜日 10時27分32秒 UTC+9 Mukut:

Dear Ohbuchi san,

Thanks for your valuable help. Yes I have defined each domain as you have said in toposetdic. I have attached following files:
outline of flow domain, blockmeshdict and toposetdic.
Please have a look.

blockMeshDict:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
    ( 0    -0.02  -0.01)
    ( 0.03 -0.02  -0.01)
    ( 0.03  0.02  -0.01)
    ( 0     0.02  -0.01)
    ( 0    -0.02   0.01)
    ( 0.03 -0.02   0.01)
    ( 0.03  0.02   0.01)
    ( 0     0.02   0.01)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (60 800 10) simpleGrading (1 0.5 1)
);

edges
(
);

boundary
(
    maxY
    {
        type wall;
        faces
        (
            (3 7 6 2)
        );
    }
    minX
    {
        type patch;
        faces
        (
            (0 4 7 3)
        );
    }
    maxX
    {
        type patch;
        faces
        (
            (2 6 5 1)
        );
    }
    minY
    {
        type wall;
        faces
        (
            (1 5 4 0)
        );
    }
    minZ
    {
        type wall;
        faces
        (
            (0 3 2 1)
        );
    }
    maxZ
    {
        type wall;
        faces
        (
            (4 5 6 7)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //

topoSetDict

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;

}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
    // Heater as dielectric 
    {
        name    heater;

        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {

            box (0 -0.00025 -0.01 )(0.002 0.00025 0.01);
        }
    }
    {
        name    heater;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (0.002 0.00005 -0.01)(0.007 0.00025 0.01);
        }
    }
    {
        name    heater;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (0.002 -0.00025 -0.01)(0.007 -0.00005 0.01);
        }
    }
    {
        name    heater;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (0.007 -0.00025 -0.01 )(0.03 0.00025 0.01);
        }
    }
    {
        name    heater;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set heater;           // name of cellSet
        }
    }

    // leftSolid as top electrode
    {
        name    leftSolid;

        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {

            box (0 0.00025 -0.01 )(0.002 0.00035 0.01);
        }
    }
    {
        name    leftSolid;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set leftSolid;
        }
    }

    // rightSolid as bottom electrode
    {
        name    rightSolid;

        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {

            box (0 -0.00035 -0.01 )(0.002 -0.00025 0.01);
        }
    }
    {
        name    rightSolid;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set rightSolid;
        }
    }

    // covered electrode as innerElec
    {

        name    innerelec;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {

            box (0.002 -0.00005 -0.01 )(0.007 0.00005 0.01);
        }
    }
    {

        name    innerelec;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set innerelec;
        }
    }
    // topAir
    {
        name    topAir;

        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {

            box (0 0.00035 -0.01 )(0.002 0.02 0.01);
        }
    }
    {
        name    topAir;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (0.002 0.00025 -0.01)(0.03 0.02 0.01);
        }
    }
    {
        name    topAir;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set topAir;
        }
    }


    // bottomAir is all the other cells
    {
        name    bottomAir;
        type    cellZoneSet;
        action  clear;
    }
    {
        name    bottomAir;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set heater;
        }
    }
    {
        name    bottomAir;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set leftSolid;
        }
    }
    {
        name    bottomAir;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set rightSolid;
        }
    }
    {
        name    bottomAir;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set topAir;
        }
    }
    {
        name    bottomAir;
        type    cellSet;
        action  invert;
    }
    {
        name    bottomAir;

        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {

            set bottomAir;
        }
    }
);

// ************************************************************************* //

Thanking you.

Mukut

 

[Mukut]

Dear Ohbuchi San,

Thank you so much. It works now. Both in /0 and /system directory folders were created for each region like bottomAir, heater, inerelce, leftSolid, rightSolid, topAir and bottomAir

but when I execute following command in terminal

decomposePar -allRegions

Following error has been found:

FOAM FATAL IO ERROR: cannot find file

file: /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/system/innerElec/decomposeParDict at line 0.

From function regIOobject::readStream() in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

I checked the directory, there is no decomposeParDict in /innerelec/ but other region folders have this file.

Actually I am following this order of command:

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite
decomposePar -allRegions
reconstructPar -allRegions
echo paraFoam -touchAll

is this okey?

Best regards,

Mukut

[ohbuchi]

To conduct parallel computation, we need decompose computational domain using
decomposePar utility.
And we should setup how to decompose via decomposeParDict.

Just copy the decomposeParDict of multiRegionHeater tutorial to your case directory.
In this tutorial, number of sub-domains is 4. So following commands would be needed .
 
>decomposePar -allRegions
>mpirun -np 4 chtMultiRegionFoam -parallel
>reconstructPar -allRegions
 


2013年10月10日木曜日 14時20分21秒 UTC+9 Mukut:

[Mukut]

Thanks.

I coppied decomposeParDict to

system/innerelec/

but same error....

Again when I execute following command:

mpirun -np 4 chtMultiRegionFoam -parallel

again error recurred and foam exit

I have attached the terminal text for your kind attention.

[ohbuchi]

The error message was changed to "already exist processor directories".

So, first of all, you should remove processor0-3 directories.

Then please try following command.

>decomposePar -allRegions

2013年10月10日木曜日 16時49分12秒 UTC+9 Mukut:

[Mukut]

Good morning Mr. Ohbuchi,

I am out of lab, after lunch I will follow your instruction and report you back

thanks

[nakagawa]

Hi, Mukut

OpenFOAM is case-sensitive.

There is "innerElec" in error message,

but "innerelec" in toposetDict.

they should be the same name, isn't it?

good luck,

nakagawa

2013年10月10日木曜日 16時49分12秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

Good afternoon. Actually after removing processor0-3 directories the problem was remain same. But It was solved after receiving reply from Mr. nakagawa, now decomperPer -all regions works

Then I try to run following command

reconstructPar -allRegions

but error occurred.....

from terminal, it said that

FOAM FATAL ERROR:
no times selected


What should I do in this steps?


Thanks.

On Thursday, October 10, 2013 7:14:44 PM UTC+9, ohbuchi wrote:

[Mukut]

Dear Nakagawa san,

Thanks a lot. After your reply I have corrected the region name in region properties dict. Now there is no error by executing following command
decomposePar -allRegions

But after that when I execute following command
reconstructPar -allRegions

In terminal following error is found

FOAM FATAL ERROR
No times selected

I didn't change anything in reconstuctPar.C

What should I do?

Thanks

Best Regards
Mukut

[nakagawa]

Mukut san,

Did you execute chtMultiRegionFoam solver itself?

> mpirun -np 4 chtMultiRegionFoam -parallel

this line is from Ohbuchi-san's comment.

nakagawa

2013年10月11日金曜日 15時57分22秒 UTC+9 Mukut:

[Mukut]

Dear Nakagawa san,

Good morning. Today I have start from the beginning and executed command manually one by one as follows:

I have deleted processor 0-3 directories before executing following commands...

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite
decomposePar -allRegions

mpirun -np 4 chtMultiRegionFoam -parallel

After this stage I found following error in terminal..

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$
 mpirun -np 4 chtMultiRegionFoam -parallel
/*---------------------------------------------------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionFoam -parallel
Date   : Oct 12 2013
Time   : 09:50:20
Host   : "mukut-Endeavor-MR3300"
PID    : 4482
Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
nProcs : 4
Slaves : 
3
(
"mukut-Endeavor-MR3300.4483"
"mukut-Endeavor-MR3300.4484"
"mukut-Endeavor-MR3300.4485"
)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

Create solid mesh for region leftSolid for time = 0

Create solid mesh for region rightSolid for time = 0

Create solid mesh for region innerelec for time = 0

*** Reading fluid mesh thermophysical properties for region bottomAir

    Adding to thermoFluid

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

    Adding to rhoFluid
[2] #0  
    Adding to UFluid

    Adding to phiFluid

Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[2]
 #3  Foam::heRhoThermo<Foam::rhoThermo, 
Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie>
 >, Foam::sensibleEnthalpy> > > >::calculate() in 
"/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2]
 #4  
Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo,
 
Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie>
 >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh 
const&, Foam::word const&) in 
"/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2]
 #5  Foam::autoPtr<Foam::rhoThermo> 
Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, 
Foam::word const&) in 
"/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2]
 #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word 
const&) in 
"/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2] #7  
[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"
[2] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #9  
[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam"
[mukut-Endeavor-MR3300:04484] *** Process received signal ***
[mukut-Endeavor-MR3300:04484] Signal: Floating point exception (8)
[mukut-Endeavor-MR3300:04484] Signal code:  (-6)
[mukut-Endeavor-MR3300:04484] Failing at address: 0x3e800001184
[mukut-Endeavor-MR3300:04484] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f05aec694a0]
[mukut-Endeavor-MR3300:04484] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f05aec69425]
[mukut-Endeavor-MR3300:04484] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f05aec694a0]
[mukut-Endeavor-MR3300:04484]
 [ 3] 
/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd)
 [0x7f05b3ccbdad]
[mukut-Endeavor-MR3300:04484] [ 4] 
/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c)
 [0x7f05b3ceba6c]
[mukut-Endeavor-MR3300:04484] [ 5] 
/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b)
 [0x7f05b3cabccb]
[mukut-Endeavor-MR3300:04484] [ 6] 
/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9)
 [0x7f05b3caa1d9]
[mukut-Endeavor-MR3300:04484] [ 7] chtMultiRegionFoam() [0x423ff8]
[mukut-Endeavor-MR3300:04484] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f05aec5476d]
[mukut-Endeavor-MR3300:04484] [ 9] chtMultiRegionFoam() [0x42c5ed]
[mukut-Endeavor-MR3300:04484] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 2 with PID 4484 on node mukut-Endeavor-MR3300 exited on signal 8 (Floating point exception).

But don't understand about this error.

Sincerely

Mukut

[Mukut]

Hi everyboday,

Good morning. By googling I came to know this error is occurred due to division by zero

But I don't understand how can I fix it. Hope to hear something from Mr. Ohbuchi and Mr. Nakagawa

Best regards.
Mukut

[ohbuchi]

Hi, Mukut-san

This error message is about the thermophysical model for fluid region.

Please check your files "constant/thermophysicalProperties" in topAir and bottomAir regions.

M.Ohbuchi

2013年10月16日水曜日 8時53分32秒 UTC+9 Mukut:

[Mukut]

Hello Ohbuchi San,

The thermophyscial properties of topAir and bottomAir was unchanged as it is in multiRegionHeater tutorial which is as follows for both in "constant/thermophysicalProperties"

mixture
{
    specie
    {
        nMoles          1;
        molWeight       28.9;
    }
    thermodynamics
    {
        Cp              1000;
        Hf              0;
    }
    transport
    {
        mu              1.8e-05;
        Pr              0.7;
    }
}

I have changed the thermophysical properties of following regions according to their properties:

heater as dielectric. This dielectric material is made from kapton film which is a polyimide and I inserted the properties of
polyimide in "constant/thermophysicalProperties" as follows:

mixture
{
    specie
    {
        nMoles      1;
        molWeight   50000;
    }

    transport
    {
        kappa   0.52;
    }

    thermodynamics
    {
        Hf      0;
        Cp      1150;
    }

    equationOfState
    {
        rho     1430;
    }
}

leftSolid, rightSolid and innerelec act as electrode which are copper electrodes and hence I used the thermophysical properties of copper for each like as bellow in "constant/thermophysicalProperties"

mixture
{
    specie
    {
        nMoles      1;
        molWeight   63.5;
    }

    transport
    {
        kappa   401;
    }

    thermodynamics
    {
        Hf      0;
        Cp      385;
    }

    equationOfState
    {
        rho     8940;
    }
}

Best regards,

Mukut

[ohbuchi]

Hi, Mukut-san,

This error would be caused by rhoThermo model for fluid region, so please check your initial value settings in 0/p file.
If the initial value of p is equal 0, floating point exception will be caused.

Masashi Obuchi


2013年10月16日水曜日 10時25分07秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi San,

The value was not zero.

Here it is:

imensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e5;

boundaryField
{
    ".*"
    {
        type            calculated;
        value           uniform 1e5;

[ohbuchi]

Hi, Mukut-san

It's difficult problem.
In the same reason, T, p, p_rgh and alphat must not zero for initial value settings.
Can you attach your case archive in tar.gz format?
I will try your settings in my OpenFOAM environment and check it.

M.Ohbuchi

2013年10月16日水曜日 13時48分35秒 UTC+9 Mukut:

[Mukut]

Thank you, I sent it

[ohbuchi]

Hi, Mukut-san

In your Allrun file,  following modification would be needed.

# remove fluid fields from solid regions (important for post-processing)
for i in heater leftSolid rightSolid   <== add "innerelec"
do
   rm -f 0*/$i/{mut,alphat,epsilon,k,U,p_rgh}
done

for i in bottomAir topAir heater leftSolid rightSolid <== add "innerelec"
do
   changeDictionary -region $i > log.changeDictionary.$i 2>&1
done

"system/innerelec/changeDictionaryDict" would be as follows;

dictionaryReplacement
{
    boundary
    {
        minY
        {
            type            patch;
        }
        minZ
        {
            type            patch;
        }
        maxZ
        {
            type            patch;
        }
    }

    T
    {
        internalField   uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
                value           uniform 300;
            }
            "innerelec_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           solidThermo;
                kappaName       none;
                value           uniform 300;
            }
            minY
            {
                type            fixedValue;
                value           uniform 500;
            }
        }
    }
}


M.Obuchi


2013年10月16日水曜日 14時38分38秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

Thanks for your continuous cooperation. I didn't use Allrun script as someone [in open-cfd forum] suggested me to run all the command manually to keep in mind the every steps.

Anyway, I have modified the Allrun script according to your suggestion and also create
system/innerelec/changeDictionaryDict
as you have told.

After executing Allrun script the terminal is as follows:

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ ./Allrun
Running blockMesh on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running topoSet on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running splitMeshRegions on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running decomposePar on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running chtMultiRegionFoam in parallel on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater using 4 processes
Running reconstructPar on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater

creating files for paraview post-processing

created 'multiRegionHeater.blockMesh'
created 'multiRegionHeater.OpenFOAM'
created 'multiRegionHeater{bottomAir}.OpenFOAM'
created 'multiRegionHeater{heater}.OpenFOAM'
created 'multiRegionHeater{innerelec}.OpenFOAM'
created 'multiRegionHeater{leftSolid}.OpenFOAM'
created 'multiRegionHeater{rightSolid}.OpenFOAM'
created 'multiRegionHeater{topAir}.OpenFOAM'

But there is no output folder based on each time interval set in controlDict files....

Please checked the attached images.
In tutorial case after the execution of Allrun script 1-10 folders were created as mentioned in controlDict but in my case, those folders are absent.

I also tried to run manually each command as follows:

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite 
decomposePar -allRegions
mpirun -np 4 chtMultiRegionFoam -parallel

but after this, same error appeared.....

Best regards,

mukut

[ohbuchi]

Hi, Mukut-san

I've attached modified archive file.

In this case, no error has occurred.

Please try this.

M.Obuchi

2013年10月16日水曜日 16時29分31秒 UTC+9 Mukut:

[Mukut]

Hi,

Did you get output folder for each time step? I didn't find......The case that I have sent to you I can open in paraFoam, but when I ran your archives and run paraFoam it shows error: here is the terminal text:

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ ./Allrun
blockMesh already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
topoSet already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
splitMeshRegions already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
decomposePar already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
chtMultiRegionFoam already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
reconstructPar already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run

creating files for paraview post-processing

created 'multiRegionHeater.blockMesh'
created 'multiRegionHeater.OpenFOAM'
created 'multiRegionHeater{bottomAir}.OpenFOAM'
created 'multiRegionHeater{heater}.OpenFOAM'
created 'multiRegionHeater{innerelec}.OpenFOAM'
created 'multiRegionHeater{leftSolid}.OpenFOAM'
created 'multiRegionHeater{rightSolid}.OpenFOAM'
created 'multiRegionHeater{topAir}.OpenFOAM'

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ ./Allclean
Cleaning /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater case

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ ./Allrun
Running blockMesh on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running topoSet on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running splitMeshRegions on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running decomposePar on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
Running chtMultiRegionFoam in parallel on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater using 4 processes
Running reconstructPar on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater

creating files for paraview post-processing

created 'multiRegionHeater.blockMesh'
created 'multiRegionHeater.OpenFOAM'
created 'multiRegionHeater{bottomAir}.OpenFOAM'
created 'multiRegionHeater{heater}.OpenFOAM'
created 'multiRegionHeater{innerelec}.OpenFOAM'
created 'multiRegionHeater{leftSolid}.OpenFOAM'
created 'multiRegionHeater{rightSolid}.OpenFOAM'
created 'multiRegionHeater{topAir}.OpenFOAM'

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ cd
mukut@mukut-Endeavor-MR3300:~$ run
mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run$ cd tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ ./Allrun
blockMesh already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
topoSet already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
splitMeshRegions already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
decomposePar already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run
chtMultiRegionFoam already run on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater: remove log file to re-run

Running reconstructPar on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater

creating files for paraview post-processing

created 'multiRegionHeater.blockMesh'
created 'multiRegionHeater.OpenFOAM'

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater$ paraFoam
ERROR: In /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/applications/utilities/postProcessing/graphics/PV3Readers/PV3FoamReader/PV3FoamReader/vtkPV3FoamReader.cxx, line 216
vtkPV3FoamReader (0x275add0): could not find valid OpenFOAM mesh


ERROR: In /home/opencfd/OpenFOAM/ThirdParty-2.1.x/ParaView-3.12.0/VTK/Filtering/vtkExecutive.cxx, line 756
vtkPVCompositeDataPipeline (0x275bff0): Algorithm vtkPV3FoamReader(0x275add0) returned failure for request: vtkInformation (0x26e6ff0)
  Debug: Off
  Modified Time: 73630
  Reference Count: 1
  Registered Events: (none)
  Request: REQUEST_INFORMATION
  ALGORITHM_AFTER_FORWARD: 1
  FORWARD_DIRECTION: 0




Segmentation fault (core dumped)


Best regard,

Mukut

[Mukut]

Sorry,

I included also my part of command in tunnel. I have run your sending case and terminal output is here:

mukut@mukut-Endeavor-MR3300:~/

[ohbuchi]

log.* files are just for reference. Please compare with your case.

And before you try Allrun script, please remove all log.* files.

M.Ohbuchi

2013年10月16日水曜日 19時04分07秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

I have checked your log files with my case. I didn't find log.reconstructPar in your archive that you sent to me, but this files in present in my case.

After removing log files I have run your archives and this time log.reconstructPar file is found and both this log files is same as my case. It includes error....

Here it is:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d

Exec   : reconstructPar -allRegions
Date   : Oct 16 2013
Time   : 19:53:41
Host   : "mukut-Endeavor-MR3300"
PID    : 5013
Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
nProcs : 1

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

--> FOAM FATAL ERROR:
No times selected

    From function reconstructPar
    in file reconstructPar.C at line 178.

FOAM exiting

========================

When you ran this case in your PC did you get output folder for each time step? Still those folders are missing both in my case and you sending case.

Sincerely

[nakagawa]

hi Mukut,

when you decompose your case, OpenFOAM creates processor* directories.

when you run multiRegionHeater using 4 processes, OpenFOAM stores results from each processors into those processor* directories.

when you reconstruct your case, OpenFOAM combines information from processor* and create time directories you want.

Please look into processor* directories after multiRegionHeater.

Are there any time directories?

if not, check log files created before the multiRegionHeater.

it is good idea to read each log files and to see which files/directories is created when you execute each command/utilities. i think.

we have to learn what we/openfoam did step by step.

nakagawa

2013年10月16日水曜日 20時14分54秒 UTC+9 Mukut:

[Mukut]

Good morning Mr. Nakagawa,

I got same advice from openfoam (cfd-online) forum to run manually each command one by one. If I execute each command how can I get the logfile for each command? Because only when I use allrun script then log files are created. What is the command to create log file?

I will return to lab within an hour and will check the processor directories for time directories/

Thank you, best regards

[ohbuchi]

Hi, Mukut-san

In the Allrun script, "runApprication blockMesh" has equal meaning to command "blockMesh > log.blockMesh".

And "runParallel `getApplication` 4" equal to "mpirun -np 4 chtMultiRegionFoam -parallel > log.chtMultiRegionFoam".

"runApplication" and "runParallel" are definded in $WM_PROJECT_DIR/bin/tools/RunFunctions.


M.Obuchi


2013年10月17日木曜日 7時27分54秒 UTC+9 Mukut:

[Mukut]

Thanks both of you.

I understand about log files now.

I have checked all the log files, all are ok except log.reconstructPar
This log files showed the error that no time is set,

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



--> FOAM FATAL ERROR:
No times selected

    From function reconstructPar
    in file reconstructPar.C at line 178.

FOAM exiting

I also checked both my case and that one sent by Ohbuchi san, in processor 0-3 directories there are only /0 and /constant directories but no time directories.

Best regards
mukut

[Mukut]

I missed this one. I also found errors in log.chtMultiRegionFoam

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d

Exec   : chtMultiRegionFoam -parallel
Date   : Oct 16 2013
Time   : 19:52:27
Host   : "mukut-Endeavor-MR3300"
PID    : 4998

Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater
nProcs : 4
Slaves : 
3
(

"mukut-Endeavor-MR3300.4999"
"mukut-Endeavor-MR3300.5000"
"mukut-Endeavor-MR3300.5001"

)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

Create solid mesh for region leftSolid for time = 0

Create solid mesh for region rightSolid for time = 0

Create solid mesh for region innerelec for time = 0

*** Reading fluid mesh thermophysical properties for region bottomAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding turbulence 

Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid

    Adding fvOptions

No finite volume options present

*** Reading fluid mesh thermophysical properties for region topAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding turbulence 

Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none
    Adding to KFluid

    Adding to dpdtFluid

    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region heater

    Adding to thermos

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

    Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region leftSolid

    Adding to thermos

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

    Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region rightSolid

    Adding to thermos

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

    Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
    Adding fvOptions

No finite volume options present

*** Reading solid mesh thermophysical properties for region innerelec

    Adding to thermos

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

    Adding to radiations

Selecting radiationModel opaqueSolid
Selecting absorptionEmissionModel constantAbsorptionEmission
Selecting scatterModel none
    Adding fvOptions

No finite volume options present

Region: bottomAir Courant Number mean: 1.9666549 max: 2
Region: topAir Courant Number mean: 19.999126 max: 20
Region: heater Diffusion Number mean: 0.00022450312 max: 0.00061033463
Region: leftSolid Diffusion Number mean: 0.072606666 max: 0.22526732
Region: rightSolid Diffusion Number mean: 0.072929511 max: 0.2229344
Region: innerelec Diffusion Number mean: 0.064452378 max: 0.22409782
deltaT = 0.0014992504
Region: bottomAir Courant Number mean: 0.029485081 max: 0.029985007
Region: topAir Courant Number mean: 0.29983698 max: 0.29985007
Region: heater Diffusion Number mean: 3.3658639e-06 max: 9.1504442e-06
Region: leftSolid Diffusion Number mean: 0.0010885557 max: 0.0033773211
Region: rightSolid Diffusion Number mean: 0.001093396 max: 0.0033423448
Region: innerelec Diffusion Number mean: 0.00096630253 max: 0.0033597874
deltaT = 0.0014992504
Time = 0.00149925


Solving for fluid region bottomAir
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 5.0773021e-08, No Iterations 13
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 2.5623023e-08, No Iterations 13
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 3.7869318e-08, No Iterations 15
DILUPBiCG:  Solving for h, Initial residual = 0.99015414, Final residual = 9.7782468e-08, No Iterations 16
Min/max T:300 300
GAMG:  Solving for p_rgh, Initial residual = 0.97866504, Final residual = 0.0085348502, No Iterations 18
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 2.8862353e-05, global = -8.9516267e-08, cumulative = -8.9516267e-08
GAMG:  Solving for p_rgh, Initial residual = 0.75632361, Final residual = 1.4420983e-07, No Iterations 1000
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (bottomAir): sum local = 7.7449257e-10, global = -1.0305277e-11, cumulative = -8.9526572e-08

Solving for fluid region topAir
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 9.403127e-08, No Iterations 17
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 9.244781e-08, No Iterations 20
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 2.3625346e-08, No Iterations 9
DILUPBiCG:  Solving for h, Initial residual = 0.99999737, Final residual = 9.2779932e-08, No Iterations 19
Min/max T:299.99998 300
GAMG:  Solving for p_rgh, Initial residual = 0.94264535, Final residual = 0.0085984122, No Iterations 51
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (topAir): sum local = 0.00012270725, global = 1.9333605e-05, cumulative = 1.9333605e-05
GAMG:  Solving for p_rgh, Initial residual = 0.20630868, Final residual = 0.00027223865, No Iterations 100
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors (topAir): sum local = 1.3535916e-05, global = 3.4963065e-06, cumulative = 2.2829912e-05

Solving for solid region heater
DICPCG:  Solving for h, Initial residual = 0.9685359, Final residual = 7.7400529e-08, No Iterations 2
DICPCG:  Solving for h, Initial residual = 0.0040168109, Final residual = 1.9928523e-09, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300

Solving for solid region leftSolid
DICPCG:  Solving for h, Initial residual = 0.99064731, Final residual = 1.1408341e-07, No Iterations 10
DICPCG:  Solving for h, Initial residual = 0.0066794438, Final residual = 5.5028158e-07, No Iterations 6
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300

Solving for solid region rightSolid
DICPCG:  Solving for h, Initial residual = 0.55693582, Final residual = 2.0094407e-07, No Iterations 9
DICPCG:  Solving for h, Initial residual = 0.48904154, Final residual = 1.9376854e-07, No Iterations 9
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300

Solving for solid region innerelec
[0] [3] [2] [1] 

[3] 
[3] --> FOAM FATAL IO ERROR: 
[3]
 keyword PIMPLE is undefined in dictionary 
"/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor3/system/innerelec/fvSolution"
[3] 
[3]
 file: 
/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor3/system/innerelec/fvSolution
[3] 
[3]     From function dictionary::subDict(const word& keyword) const
[3]     in file db/dictionary/dictionary.C at line 608.
[3] 
FOAM parallel run exiting
[3] 


[0] 
[0] --> FOAM FATAL IO ERROR: 
[0]
 keyword PIMPLE is undefined in dictionary 
"/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor0/system/innerelec/fvSolution"
[0] 
[0]
 file: 
/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor0/system/innerelec/fvSolution
[0] 
[0]     From function dictionary::subDict(const word& keyword) const
[0]     in file db/dictionary/dictionary.C at line 608.
[0] 
FOAM parallel run exiting
[0] 
[2] [1] 
[1] --> FOAM FATAL IO ERROR: 
[1]
 keyword PIMPLE is undefined in dictionary 
"/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor1/system/innerelec/fvSolution"
[1] 
[1]
 file: 
/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor1/system/innerelec/fvSolution
[1] 
[1]     From function dictionary::subDict(const word& keyword) const
[1]     in file db/dictionary/dictionary.C at line 608.
[1] 
FOAM parallel run exiting
[1] 

[2] --> FOAM FATAL IO ERROR: 
[2]
 keyword PIMPLE is undefined in dictionary 
"/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor2/system/innerelec/fvSolution"
[2] 
[2]
 file: 
/home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater/processor2/system/innerelec/fvSolution
[2] 
[2]     From function dictionary::subDict(const word& keyword) const
[2]     in file db/dictionary/dictionary.C at line 608.
[2] 
FOAM parallel run exiting
[2] 
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 0 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.
--------------------------------------------------------------------------
--------------------------------------------------------------------------
mpirun has exited due to process rank 3 with PID 5001 on
node mukut-Endeavor-MR3300 exiting without calling "finalize". This may
have caused other processes in the application to be
terminated by signals sent by mpirun (as reported here).
--------------------------------------------------------------------------
[mukut-Endeavor-MR3300:04997] 3 more processes have sent help message help-mpi-api.txt / mpi-abort
[mukut-Endeavor-MR3300:04997] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

[Mukut]

After checking /system/regionName/fvSolution, I found the difference in /system/innerelec/fvSolution


This is for leftSolid
/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;

    object      fvSolution;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    h
    {
        solver           PCG;
        preconditioner   DIC;
        tolerance        1e-06;
        relTol           0.1;
    }

    hFinal
    {
        $h;
        tolerance        1e-06;
        relTol           0;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 1;
}

// ************************************************************************* //

but the difference is here for innerelec

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      binary;
    class       dictionary;
    location    "system/innerelec";
    object      fvSolution;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// ************************************************************************* //

I now copy those missing lines here, and after running the allrun script I will inform again

[ohbuchi]

Hi, Mukut-san

reconstructPar is a utility for recombining regions after parallel computation, so before using it, you should complete paralell simulation.
And my archive file has following mistakes, please modify it by yourself.

syste/innerelec/fvSolution, fvSchemes are empty, please copy from system/heater.

M.Obuchi


2013年10月17日木曜日 8時54分25秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

I have changed the fvSchemes and fvSolutions for innerelec....

Now Allrun script is running......already 30mins gone, hope this time it will work properly.

in terminal following information is displayed

Running chtMultiRegionFoam in parallel on /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionFoam/multiRegionHeater using 4 processes

I will inform after finishing the simulation. May be next time I need to reduce time in controlDict file to save time in this stage.

Best regards

[ohbuchi]

Hi, Mukut-san

Because the value of WriteInterval in your controlDict is relatively large 1.0,  long times would be needed for making first time directory in processor directories.
To check whether the simulation is running how much,  please enter the following command.
>tail -n 100 log.chtMultiRegionFoam


M.Ohbuchi

[Mukut]

Hi Ohbuchi san,

here it is>>

Region: bottomAir Courant Number mean: 0.0011865337 max: 0.0042069857
Region: topAir Courant Number mean: 0.11624907 max: 0.29504471
Region: heater Diffusion Number mean: 4.6473463e-07 max: 1.2634285e-06
Region: leftSolid Diffusion Number mean: 0.00015030006 max: 0.00046631656
Region: rightSolid Diffusion Number mean: 0.00015096837 max: 0.00046148728
Region: innerelec Diffusion Number mean: 0.0001334202 max: 0.00046389564
deltaT = 0.00021046409
Time = 0.0175536

May be I should stop the simulation and make  end time 0.2 with time step 0.1

[Mukut]

Now Time = 0.0312073

So, It will take much more times, I think whole day is not enough. How to stop this simulation without shut down PC? I should reduce the time.

[Mukut]

I have killed the simulation process because it takes long time....

I have changed the controlDict like as follows:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;

    location    "system";
    object      controlDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

libs
(
    "libcompressibleTurbulenceModel.so"
    "libcompressibleRASModels.so"
);

application     chtMultiRegionFoam;

startFrom       latestTime;

startTime       0.1;

stopAt          endTime;

endTime         0.2;

deltaT          0.1;

writeControl    adjustableRunTime;

writeInterval   0.1;

purgeWrite      0;

writeFormat     binary;

writePrecision  8;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;

maxCo           0.3;

// Maximum diffusion number
maxDi           10.0;

adjustTimeStep  yes;

// ************************************************************************* //

But it takes time....how can I reduce the simulation time?

[Mukut]

Dear Obuchi and Nakagawa san,

Good morning. The simulation takes long time, after whole night simulation time showed 0.12 where as it will stop at 0.2. I already reduce the end time and write interval, but it is not satisfactorily reduce the time of simulation. How can I reduce the time of simulation?

Best regards,

[ohbuchi]

Hi, Mukut-san

The solver chtMultiRegionFoam uses PIMPLE algorithm, so you can set larger Co, like 1.0.
For using large Co number in PIMPLE, you should set cOuterCorrectors >>1.
And if you don't interest in transient variation of the solution fields, you should use chtMultiRegionSimpleFoam.

M.Ohbuchi


2013年10月18日金曜日 8時52分31秒 UTC+9 Mukut:

[Mukut]

Thank you Ohbuchi san,

In which file, shall I have to set cOuterCorrectors >>1?

Yup, it is better to use steady case of chtMultiRegionSimpleFoam.

Best regards

[ohbuchi]

The parameter "nOuterCorrectors" is in PIMPLE section of "system/fvSolution".
If nOuterCorrectors equals to 1, PIMPLE algorithm would be same as PISO.


2013年10月18日金曜日 10時03分26秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi San,

Thank you. In sytem/fvSolution, I have found that nOuterCorrectors is 1, is there any rule to increase this value? or I just arbitrarily choose?

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;

    object      fvSolution;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

PIMPLE
{
    nOuterCorrectors 1;
}

// ************************************************************************* //

but in chtMultiRegionSimpleFoam, there is no info about nOuterCorrectors which is as follows...

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;

    object      fvSolution;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// ************************************************************************* //

Now simulation time is Time = 0.141968

After finishing I will shit to chtMultiRegionSimpleFoam

[ohbuchi]

The parameter "nOuterCorrectors" is number of outer loop of PIMPLE, please try nOuterCorrectors=2~10.
For large Co, nOuterCorrectors should be larger.

The "chtMultiRegionSimpleFoam" is steady-state solver using SIMPLE algorithm, so it doesn't need outer loop.

[Mukut]

Thank you so much, I understand now. My professor also told me to simulate as a steady case, later if necessary we have to introduce transient flow....

I just wait for the ending of simulation, within 1hrs it will finish, if this time time directory is created then I will proceed for steady state case

Thanks for your long way of cooperation and if I face further problem, I will knock you

Best regards
Mukut

[Mukut]

Dear Ohbuchi and Nakagawa san,

Finally the simulation has been finished and I found the time directory. So, tomorrow I will use chtMultiRegionSimpleFoam.

I need one suggestion, I want to define each region as a block in blockMeshDict file, also each regions will be defined by topoSet as usual...so that I can choose different mesh size for each region.... is the procedure ok? I mean I want to make this type of different mesh size, how can I do this?

Best regards,

mukut

[ohbuchi]

Congratulation!

It's my pleasure to hear your success.

Each region can be made as separate mesh.

Please see the tutorial "chtMultiRegionSimpleFoam/heatExchanger".

M.Ohbuchi

2013年10月18日金曜日 19時13分36秒 UTC+9 Mukut:

[Mukut]

Thank you so much. Tomorrow I will check it :)

On Friday, October 18, 2013 9:55:58 PM UTC+9, ohbuchi wrote:

Congratulation!

It's my pleasure to hear your success.

Each region can be made as separate mesh.

Please see the tutorial "chtMultiRegionSimpleFoam/heatExchanger".

M.Ohbuchi

2013年10月18日金曜日 19時13分36秒 UTC+9 Mukut:

Dear Ohbuchi and Nakagawa san,

Finally the simulation has been finished and I found the time directory. So, tomorrow I will use chtMultiRegionSimpleFoam.

I need one suggestion, I want to define each region as a block in blockMeshDict file, also each regions will be defined by topoSet as usual...so that I can choose different mesh size for each region.... is the procedure ok? I mean I want to make this type of different mesh size, how can I do this?

Best regards,

mukut

On Friday, October 18, 2013 2:08:56 PM UTC+9, Mukut wrote:

Thank you so much, I understand now. My professor also told me to simulate as a steady case, later if necessary we have to introduce transient flow....

[Mukut]

Good morning Mr. Ohbuchi and Mr. Nakagawa,

This morning I have shifted my case from transient to steadystate condition. So, I have modified the tutorial of multiRegioneHeater of chtMultiRegionSimpleFoam.....

I have modified blockMesh, topoSetDict,Allrun Script and for innerElec I have changed fvSchemes, fvSolution and changeDictionaryDict

After excecuting Allrun Script all regions are created including new region innerElec... but there were no processor 0~3 directories....

I have checked all the logfiles and found error in log.chtMultiRegionSimpleFoam as follows:

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 19 2013
Time   : 10:52:49
Host   : "mukut-Endeavor-MR3300"
PID    : 4046
Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater

nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

--> FOAM FATAL IO ERROR: 

keyword startFace is undefined in dictionary ".minY"

file: .minY from line 111 to line 111.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 402.

FOAM exiting

But when I execute each command manually like as follows:

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite
decomposePar -allRegions

mpirun -np 4 chtMultiRegionFoam -parallel

In this case processor0~3 directories have been created but following error displayed in the terminal:

mukut@mukut-Endeavor-MR3300:~/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater$ mpirun -np 4 chtMultiRegionSimpleFoam -parallel
/*---------------------------------------------------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam -parallel
Date   : Oct 19 2013
Time   : 10:56:09
Host   : "mukut-Endeavor-MR3300"
PID    : 4086
Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater

nProcs : 4
Slaves : 
3
(

"mukut-Endeavor-MR3300.4087"
"mukut-Endeavor-MR3300.4088"
"mukut-Endeavor-MR3300.4089"

)

Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0

sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

Create solid mesh for region leftSolid for time = 0

Create solid mesh for region rightSolid for time = 0

Create solid mesh for region innerElec for time = 0

*** Reading fluid mesh thermophysical properties for region bottomAir

    Adding to thermoFluid

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

[1] #0  [3] #0  [0] [2] #0  #0  Foam::error::printStack(Foam::Ostream&)Foam::error::printStack(Foam::Ostream&)Foam::error::printStack(Foam::Ostream&)Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #1   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #1  Foam::sigFpe::sigHandler(int)Foam::sigFpe::sigHandler(int) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[3] #2   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[0] #2   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[2] #2   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
[1] #2   in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[1] #4  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[3] #4  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[0] #4  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2] #4  Foam::rhoThermo::addfvMeshConstructorToTable<Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[3] #5  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[1] #5  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[0] #5  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2] #5  Foam::autoPtr<Foam::rhoThermo> Foam::basicThermo::New<Foam::rhoThermo>(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[3] #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[1] #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[0] #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2] #6  Foam::rhoThermo::New(Foam::fvMesh const&, Foam::word const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[3] #7   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[1] #7   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[2] #7   in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
[0] #7  



[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[2] #8  __libc_start_main[3]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[3] #8  __libc_start_main[0]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[0] #8  __libc_start_main[1]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[1] #8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
[0] #9   in "/lib/x86_64-linux-gnu/libc.so.6"
[3] #9   in "/lib/x86_64-linux-gnu/libc.so.6"
[2] #9   in "/lib/x86_64-linux-gnu/libc.so.6"
[1] #9  



[2]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[mukut-Endeavor-MR3300:04088] *** Process received signal ***
[mukut-Endeavor-MR3300:04088] Signal: Floating point exception (8)
[mukut-Endeavor-MR3300:04088] Signal code:  (-6)
[mukut-Endeavor-MR3300:04088] Failing at address: 0x3e800000ff8
[mukut-Endeavor-MR3300:04088] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f82fe46e4a0]
[mukut-Endeavor-MR3300:04088] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f82fe46e425]
[mukut-Endeavor-MR3300:04088] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f82fe46e4a0]
[mukut-Endeavor-MR3300:04088] [ 3] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd) [0x7f8301bd3dad]
[mukut-Endeavor-MR3300:04088] [ 4] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c) [0x7f8301bf3a6c]
[mukut-Endeavor-MR3300:04088] [ 5] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b) [0x7f8301bb3ccb]
[mukut-Endeavor-MR3300:04088] [ 6] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9) [0x7f8301bb21d9]
[mukut-Endeavor-MR3300:04088] [ 7] chtMultiRegionSimpleFoam() [0x421c20]
[mukut-Endeavor-MR3300:04088] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f82fe45976d]
[mukut-Endeavor-MR3300:04088] [ 9] chtMultiRegionSimpleFoam() [0x4290ed]
[mukut-Endeavor-MR3300:04088] *** End of error message ***
[0]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[mukut-Endeavor-MR3300:04086] *** Process received signal ***
[mukut-Endeavor-MR3300:04086] Signal: Floating point exception (8)
[mukut-Endeavor-MR3300:04086] Signal code:  (-6)
[mukut-Endeavor-MR3300:04086] Failing at address: 0x3e800000ff6
[mukut-Endeavor-MR3300:04086] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f7d6da274a0]
[mukut-Endeavor-MR3300:04086] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f7d6da27425]
[mukut-Endeavor-MR3300:04086] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f7d6da274a0]
[mukut-Endeavor-MR3300:04086] [ 3] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd) [0x7f7d7118cdad]
[mukut-Endeavor-MR3300:04086] [ 4] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c) [0x7f7d711aca6c]
[mukut-Endeavor-MR3300:04086] [ 5] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b) [0x7f7d7116cccb]
[mukut-Endeavor-MR3300:04086] [ 6] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9) [0x7f7d7116b1d9]
[mukut-Endeavor-MR3300:04086] [ 7] chtMultiRegionSimpleFoam() [0x421c20]
[mukut-Endeavor-MR3300:04086] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f7d6da1276d]
[mukut-Endeavor-MR3300:04086] [ 9] chtMultiRegionSimpleFoam() [0x4290ed]
[mukut-Endeavor-MR3300:04086] *** End of error message ***
[3]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[mukut-Endeavor-MR3300:04089] *** Process received signal ***
[mukut-Endeavor-MR3300:04089] Signal: Floating point exception (8)
[mukut-Endeavor-MR3300:04089] Signal code:  (-6)
[mukut-Endeavor-MR3300:04089] Failing at address: 0x3e800000ff9
[mukut-Endeavor-MR3300:04089] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f86973604a0]
[mukut-Endeavor-MR3300:04089] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f8697360425]
[mukut-Endeavor-MR3300:04089] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f86973604a0]
[mukut-Endeavor-MR3300:04089] [ 3] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd) [0x7f869aac5dad]
[mukut-Endeavor-MR3300:04089] [ 4] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c) [0x7f869aae5a6c]
[mukut-Endeavor-MR3300:04089] [ 5] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b) [0x7f869aaa5ccb]
[mukut-Endeavor-MR3300:04089] [ 6] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9) [0x7f869aaa41d9]
[mukut-Endeavor-MR3300:04089] [ 7] chtMultiRegionSimpleFoam() [0x421c20]
[mukut-Endeavor-MR3300:04089] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f869734b76d]
[mukut-Endeavor-MR3300:04089] [ 9] chtMultiRegionSimpleFoam() [0x4290ed]
[mukut-Endeavor-MR3300:04089] *** End of error message ***
[1]  in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
[mukut-Endeavor-MR3300:04087] *** Process received signal ***
[mukut-Endeavor-MR3300:04087] Signal: Floating point exception (8)
[mukut-Endeavor-MR3300:04087] Signal code:  (-6)
[mukut-Endeavor-MR3300:04087] Failing at address: 0x3e800000ff7
[mukut-Endeavor-MR3300:04087] [ 0] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f08ff40a4a0]
[mukut-Endeavor-MR3300:04087] [ 1] /lib/x86_64-linux-gnu/libc.so.6(gsignal+0x35) [0x7f08ff40a425]
[mukut-Endeavor-MR3300:04087] [ 2] /lib/x86_64-linux-gnu/libc.so.6(+0x364a0) [0x7f08ff40a4a0]
[mukut-Endeavor-MR3300:04087] [ 3] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11heRhoThermoINS_9rhoThermoENS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEE9calculateEv+0x6cd) [0x7f0902b6fdad]
[mukut-Endeavor-MR3300:04087] [ 4] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo27addfvMeshConstructorToTableINS_11heRhoThermoIS0_NS_11pureMixtureINS_14constTransportINS_7species6thermoINS_12hConstThermoINS_10perfectGasINS_6specieEEEEENS_16sensibleEnthalpyEEEEEEEEEE3NewERKNS_6fvMeshERKNS_4wordE+0x5c) [0x7f0902b8fa6c]
[mukut-Endeavor-MR3300:04087] [ 5] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam11basicThermo3NewINS_9rhoThermoEEENS_7autoPtrIT_EERKNS_6fvMeshERKNS_4wordE+0x11b) [0x7f0902b4fccb]
[mukut-Endeavor-MR3300:04087] [ 6] /opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so(_ZN4Foam9rhoThermo3NewERKNS_6fvMeshERKNS_4wordE+0x9) [0x7f0902b4e1d9]
[mukut-Endeavor-MR3300:04087] [ 7] chtMultiRegionSimpleFoam() [0x421c20]
[mukut-Endeavor-MR3300:04087] [ 8] /lib/x86_64-linux-gnu/libc.so.6(__libc_start_main+0xed) [0x7f08ff3f576d]
[mukut-Endeavor-MR3300:04087] [ 9] chtMultiRegionSimpleFoam() [0x4290ed]
[mukut-Endeavor-MR3300:04087] *** End of error message ***
--------------------------------------------------------------------------
mpirun noticed that process rank 0 with PID 4086 on node mukut-Endeavor-MR3300 exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------

Any suggestion???

Best regards
Mukut

[Mukut]

Dear Ohbuchi san and Nakagawa san,

I have found following dissimilarities between chtMultiRegionFoam and chtMultiRegionSimpleFoam  in boundary files at contant/heater/polymesh

Dissimilarities are shown in red color...

Format also different in both files!!!

chtMultiRegionFoam case:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      binary;

    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

9
(
minX
{
    type            patch;
    nFaces          100;
    startFace       16000;
}

maxX
{
    type            patch;
    nFaces          100;
    startFace       16100;
}

minZ
{
    type            patch;
    nFaces          580;
    startFace       16200;
}

maxZ
{
    type            patch;
    nFaces          580;
    startFace       16780;
}

heater_to_leftSolid
{
    type            mappedWall;
    nFaces          40;
    startFace       17360;
    sampleMode      nearestPatchFace;
    sampleRegion    leftSolid;
    samplePatch     leftSolid_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_innerelec
{
    type            mappedWall;
    nFaces          240;
    startFace       17400;
    sampleMode      nearestPatchFace;
    sampleRegion    innerelec;
    samplePatch     innerelec_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_rightSolid
{
    type            mappedWall;
    nFaces          40;
    startFace       17640;
    sampleMode      nearestPatchFace;
    sampleRegion    rightSolid;
    samplePatch     rightSolid_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_topAir
{
    type            mappedWall;
    nFaces          560;
    startFace       17680;
    sampleMode      nearestPatchFace;
    sampleRegion    topAir;
    samplePatch     topAir_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_bottomAir
{
    type            mappedWall;
    nFaces          560;
    startFace       18240;
    sampleMode      nearestPatchFace;
    sampleRegion    bottomAir;
    samplePatch     bottomAir_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

)


// ************************************************************************* //

chtMultiRegionSimpleFoam

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;

    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

10
(
minX
{
    type            patch;
    nFaces          100;
    startFace       16000;
}

maxX
{
    type            patch;
    nFaces          100;
    startFace       16100;
}

minZ
{
    type            patch;
    nFaces          580;
    startFace       16200;
}

maxZ
{
    type            patch;
    nFaces          580;
    startFace       16780;
}

heater_to_leftSolid
{
    type            mappedWall;
    nFaces          40;
    startFace       17360;
    sampleMode      nearestPatchFace;
    sampleRegion    leftSolid;
    samplePatch     leftSolid_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_innerElec
{
    type            mappedWall;
    nFaces          240;
    startFace       17400;
    sampleMode      nearestPatchFace;
    sampleRegion    innerElec;
    samplePatch     innerElec_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_rightSolid
{
    type            mappedWall;
    nFaces          40;
    startFace       17640;
    sampleMode      nearestPatchFace;
    sampleRegion    rightSolid;
    samplePatch     rightSolid_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_topAir
{
    type            mappedWall;
    nFaces          560;
    startFace       17680;
    sampleMode      nearestPatchFace;
    sampleRegion    topAir;
    samplePatch     topAir_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

heater_to_bottomAir
{
    type            mappedWall;
    nFaces          560;
    startFace       18240;
    sampleMode      nearestPatchFace;
    sampleRegion    bottomAir;
    samplePatch     bottomAir_to_heater;
    offsetMode      uniform;
    offset          ( 0 0 0 );
}

minY
{
    type            patch;
}

)


// ************************************************************************* //

Eagerly waiting for both of your response.

Thanks

[Mukut]

Till now I couldn't solve this issue :(
Waiting for your reply.....

Best regards
mukut

[Mukut]

Dear Ohbuchi and Nakagawa san,

If I removed the minY entry (red color) from changeDictionaryDict of heater as shown below, then previous error regarding undefined minY was disappeared.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;

    class       dictionary;
    object      changeDictionaryDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    boundary
    {
        minY
        {
            type            patch;
        }
        minZ
        {
            type            patch;
        }
        maxZ
        {
            type            patch;
        }
    }

    T
    {
        internalField   uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
                value           uniform 300;
            }
            "heater_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           solidThermo;
                kappaName       none;
                value           uniform 300;
            }
            minY
            {
                type            fixedValue;
                value           uniform 500;
            }
        }
    }
}

// ************************************************************************* //

Then following error has been found in log.chtMultiRegionSimpleFoam

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 19 2013

Time   : 17:28:47
Host   : "mukut-Endeavor-MR3300"
PID    : 10837

Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

Create solid mesh for region leftSolid for time = 0

Create solid mesh for region rightSolid for time = 0

Create solid mesh for region innerelec for time = 0

*** Reading fluid mesh thermophysical properties for region bottomAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence

Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none

    Adding fvOptions

No finite volume options present

*** Reading fluid mesh thermophysical properties for region topAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence

Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none

faceSource topAir_minX:
    total faces  = 4610
    total area   = 0.0003926898


faceSource topAir_maxX:
    total faces  = 4630
    total area   = 0.0003947585


Time = 1

Solving for fluid region bottomAir

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.0003437786, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0001685591, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.6769308, Final residual = 0.0003296941, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.7032969, Final residual = 0.009508086, No Iterations 1
Min/max T:300 300
GAMG:  Solving for p_rgh, Initial residual = 0.9845118, Final residual = 0.009485646, No Iterations 21
time step continuity errors : sum local = 0.008117152, global = -5.408644e-17, cumulative = -5.408644e-17
Min/max rho:1.158623 1.158623

Solving for fluid region topAir

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.0003068075, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.0002554454, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.8006577, Final residual = 0.0004901631, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.9994282, Final residual = 0.003423423, No Iterations 1
Min/max T:300 300
GAMG:  Solving for p_rgh, Initial residual = 0.6488513, Final residual = 0.00631892, No Iterations 46
time step continuity errors : sum local = 0.003455513, global = 0.000696638, cumulative = 0.000696638
Min/max rho:1.158623 1.158623

Solving for solid region heater

--> FOAM FATAL ERROR: 
Attempt to cast type zeroGradient to type compressible::turbulentTemperatureCoupledBaffleMixed

    From function refCast<To>(From&)
    in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.1/src/OpenFOAM/lnInclude/typeInfo.H at line 114.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::compressible::turbulentTemperatureCoupledBaffleMixedFvPatchScalarField::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so"
#3  Foam::mixedFvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::mixedEnergyFvPatchScalarField::updateCoeffs() in "/opt/openfoam221/platforms/linux64GccDPOpt/lib/libfluidThermophysicalModels.so"
#5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#6  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#7  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 in "/opt/openfoam221/platforms/linux64GccDPOpt/bin/chtMultiRegionSimpleFoam"
Aborted (core dumped)

Whole day I am trying to figure it out, but all attempts goes in vain.

Hope to get a hints/idea/solution regarding this error from you soon.

Best regard,

Mukut

[ohbuchi]

Hi, Mukut-san

Format is "ascii", if you can read in text editor. "binary" is not correct.

And in the boundary dictionary, all patch must be definded by startFace & nFaces, so in your boundary

dictionary minY is incorrect or non-exist patch. Please remove it from boundary.

M.Ohbuchi

2013年10月19日土曜日 12時51分01秒 UTC+9 Mukut:

[ohbuchi]

Hi, Mukut-san

Allrun script contain important procedure that is not included in your command input;

rm -f 0*/$i/{mut,alphat,k,epsilon,U,p_rgh}  ... for solid region

If you omit this procedure, initialization of thermo physical model for solid region would be failed

by floating point exception.

M.Ohbuchi

2013年10月19日土曜日 11時11分28秒 UTC+9 Mukut:

[Mukut]

Dear Ohbuchi san,

Thank you. But this entry was present in the same changedictionarydict file for heater in chtMultiRegionFoam,

Anyway, yes I have removed the minY entry from changedictionarydict file, then ran the allrun script but following error found in log.chtmultiRegionSimpleFoam

/*---------------------------------------------------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

Build  : 2.2.1-57f3c3617a2d
Exec   : chtMultiRegionSimpleFoam
Date   : Oct 19 2013

Time   : 17:28:47
Host   : "mukut-Endeavor-MR3300"
PID    : 10837

Case   : /home/mukut/OpenFOAM/mukut-2.2.1/run/tutorials/heatTransfer/chtMultiRegionSimpleFoam/multiRegionHeater
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Create time

Create fluid mesh for region bottomAir for time = 0

Create fluid mesh for region topAir for time = 0

Create solid mesh for region heater for time = 0

Create solid mesh for region leftSolid for time = 0

Create solid mesh for region rightSolid for time = 0

Create solid mesh for region innerelec for time = 0

*** Reading fluid mesh thermophysical properties for region bottomAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence


Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none
    Adding fvOptions

No finite volume options present

*** Reading fluid mesh thermophysical properties for region topAir

    Adding to thermoFluid

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

    Adding to rhoFluid

    Adding to UFluid

    Adding to phiFluid

    Adding to gFluid

    Adding to turbulence


Selecting turbulence model type laminar
    Adding to ghFluid

    Adding to ghfFluid

Selecting radiationModel none

- show quoted text -

[Mukut]

Dear Ohbuchi San,

In allrun script the line is present:

#!/bin/sh
cd ${0%/*} || exit 1    # run from this directory


# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions

runApplication blockMesh
runApplication topoSet
runApplication splitMeshRegions -cellZones -overwrite

# remove fluid fields from solid regions (important for post-processing)
for i in heater leftSolid rightSolid innerelec
do
   rm -f 0*/$i/{mut,alphat,epsilon,k,U,p_rgh}
done

for i in bottomAir topAir heater leftSolid rightSolid innerelec
do
   changeDictionary -region $i > log.changeDictionary.$i 2>&1
done


#-- Run on single processor
runApplication `getApplication`

## Decompose
#runApplication decomposePar -allRegions
#
## Run
#runParallel `getApplication` 4
#
## Reconstruct
#runApplication reconstructPar -allRegions


echo
echo "creating files for paraview post-processing"
echo
paraFoam -touchAll

# ----------------------------------------------------------------- end-of-file

I used allrun script and even removing minY entry from changedictionaryDict file of heater error found in log.chtMultiRegionSimpleFoam

best regard
mukut

[Mukut]

Till now I couldn't solve by myself, I eagerly waiting for your reply, please help me

[nakagawa]

hi Mukut,

the error message you got;

Solving for solid region heater

 

--> FOAM FATAL ERROR: 
Attempt to cast type zeroGradient to type compressible::turbulentTemperatureCoupledBaffleMixed

Have you checked boundary conditions throughout?

A zeroGradient condition would be used at the boundary where turbulentTemperatureCoupledBaffleMixed should be used.

the "heater" region is the highly suspicious region.

but the regions adjacent to heater are also suspicious.

The boundary condition between solid and fluid regions will have the same condition at both side (regions).

Please make sure turbulentTemperatureCoupledBaffleMixed conditions are imposed at the boundaries adjacent to the fluid region.

Unexpected emergence of minY might be related to the erroneous boundary conditions.

Please check your files without any preconceptions.

nakagawa

2013年10月22日火曜日 8時00分02秒 UTC+9 Mukut:

[Mukut]

Dear Nakagawa san,

Good morning. I didn't change any boundary condition. Last time I can run chtMultiRegionFoam successfully but why not in steady state version? I only changed blockMeshDict, topoSetDict etc in the same way that I have done in chtMultiRegionFoam.

I will check again after return to lab

Mukut

[Mukut]

Good Noon,

I have found the typing mistake in changeDictionaryDict of innerelec and after correcting, the simulation runs perfectly. But changeDictionaryDict of heater  is different from original tutorial, I have removed minY entry from this file. I have also checked that if I restored original changeDictionaryDict of heater  then following error showed in log file:

--> FOAM FATAL IO ERROR: 
keyword startFace is undefined in dictionary ".minY"

file: .minY from line 111 to line 111.

    From function dictionary::lookupEntry(const word&, bool, bool) const
    in file db/dictionary/dictionary.C at line 402.

FOAM exiting

 Tutorial changeDictionaryDict of heater is as follows:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;

    class       dictionary;
    object      changeDictionaryDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    boundary
    {
        minY
        {
            type            patch;
        }
        minZ
        {
            type            patch;
        }
        maxZ
        {
            type            patch;
        }
    }

    T
    {
        internalField   uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
                value           uniform 300;
            }
            "heater_to_.*"
            {
                type            compressible::turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           solidThermo;
                kappaName       none;
                value           uniform 300;
            }
            minY
            {
                type            fixedValue;
                value           uniform 500;
            }
        }
    }
}

// ************************************************************************* //

after removing minY entry it is as follows:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version     2.0;
    format      ascii;

    class       dictionary;
    object      changeDictionaryDict;

}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dictionaryReplacement
{
    boundary
    {

       
        minZ
        {
            type            patch;
        }
        maxZ
        {
            type            patch;
        }
    }

    T
    {
        internalField   uniform 300;

        boundaryField
        {
            ".*"
            {
                type            zeroGradient;
                value           uniform 300;
            }
            "heater_to_.*"
            {
                type            compressible::

turbulentTemperatureCoupledBaffleMixed;
                neighbourFieldName T;
                kappa           solidThermo;
                kappaName       none;
                value           uniform 300;
            }
             
        }
    }
}

// ************************************************************************* //

Now I am looking for some literatures to know how to modify fvSchemes as I have to modify heat transfer equation to electrical field solver equation. Do you have some link/book/research paper, from which I can learn?

Sincerely

[Bhargav Ajith]

hi mukut 

i have a problem running a ship simulation in openfoam,the error is while running the reconstructpar.c file.it shows an error saying " no times selected".can u  help me with it?