 |
 |
 |
|
|
|
[Sponsors] | ||||
Problem with heat source for OpenFOAM version > 2012 |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
August 2, 2024, 16:41
|
Problem with heat source for OpenFOAM version > 2012
|
#1 | |
|
Member
Nikos
Join Date: Aug 2012
Location: Greece
Posts: 30
Rep Power: 14  |
Hi all.
I am using the following code, as a fvOptions file, in order to apply a heat source in a specific domain. My solver is the chtMultiRegionSimpleFoam. I have multiple solid and fluid domains. The general workflow of the problem is: meshing->decomposePar->chtMultiRegionSimpleFoam in parallel->reconstructPar. Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
heat_source
{
type scalarCodedSource;
name sourceTerm_Wa_A;
active true;
scalarCodedSourceCoeffs
{
fields (h);
selectionMode all;
codeInclude
#{
#};
codeCorrect
#{
Pout<< "**codeCorrect**" << endl;
#};
codeAddSup
#{
const Time& time = mesh().time();
const volScalarField& Tm = mesh_.lookupObject<volScalarField>("T");
const vectorField& C = mesh_.C();
const scalarField& V = mesh_.V();
scalarField& hSource = eqn.source(); //defining source
forAll(C, i)
{
hSource[i] = Tm*V[i];
}
Pout << "***codeAddSup***" << endl;
#};
codeSetValue
#{
Pout<< "**codeSetValue**" << endl;
#};
// Dummy entry. Make dependent on above to trigger recompilation
code
#{
$codeInclude
$codeCorrect
$codeAddSup
$codeSetValue
#};
}
}
// ************************************************************************* //
Quote:
I would appreciate any feedback or advice! Thanks a lot Nikos |
||
|
|
||
|
August 2, 2024, 17:00
|
|
#2 | |
|
Member
Nikos
Join Date: Aug 2012
Location: Greece
Posts: 30
Rep Power: 14 |
I want also to add that the error persists in the case of serial running:
Quote:
Thus, it is probably not an MPI problem.. |
||
|
|
|
||
|
August 6, 2024, 12:14
|
|
#3 | ||
|
Member
Lorenzo
Join Date: Apr 2020
Location: Italy
Posts: 47
Rep Power: 6 |
Hello,
The issue seems to be in the calculation of hSource: Quote:
You can also see the error indicated in FOAM FATAL IO ERROR: Quote:
Lorenzo |
|||
|
|
|
|||
|
August 6, 2024, 13:19
|
|
#4 | |
|
Member
Nikos
Join Date: Aug 2012
Location: Greece
Posts: 30
Rep Power: 14 |
You are right. That was one problem, but not what I was looking for!
Let my explain. I have removed some terms in order to simplify the source (for demonstration reasons) and it seems that I accidentally removed also the [i] part from Tm. Thus, unfortunately, that was not my problem. The error log now is: Quote:
The (corrected) code now is: Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
heat_source
{
type scalarCodedSource;
name sourceTerm_Wa_A;
active true;
scalarCodedSourceCoeffs
{
fields (h);
selectionMode all; // all, cellSet, cellZone, points
codeInclude
#{
#};
codeCorrect
#{
Pout<< "**codeCorrect**" << endl;
#};
codeAddSup
#{
const Time& time = mesh().time();
const volScalarField& Tm = mesh_.lookupObject<volScalarField>("T");
const vectorField& C = mesh_.C(); //List of cellcentres
const scalarField& V = mesh_.V(); //Volume of an individual cell in the cellZone
scalarField& hSource = eqn.source(); //defining source
forAll(C, i)
{
hSource[i] = Tm[i]*V[i];
}
Pout << "***codeAddSup***" << endl;
#};
codeSetValue
#{
Pout<< "**codeSetValue**" << endl;
#};
// Dummy entry. Make dependent on above to trigger recompilation
code
#{
$codeInclude
$codeCorrect
$codeAddSup
$codeSetValue
#};
}
}
// ************************************************************************* //
Thanks for your reply anyway! Best regards, Nikos |
||
|
|
|
||
|
August 7, 2024, 04:39
|
|
#5 | |
|
Member
Lorenzo
Join Date: Apr 2020
Location: Italy
Posts: 47
Rep Power: 6 |
Hi,
Also my bad because I tried the corrected script only with OpenFOAM-v2012  It looks like scalarCodedSource has been modified to distinguish between incompressible and compressible cases. Have a look at this post: OF v2112: problem with twoPhaseEulerFoam & scalarCodedSource As suggested here, you could try using "codedAddSupRho" instead of "codedAddSup". I guess this is the case, we can see in chtMultiRegionSimpleFoam/fluid/EEqn.H that the source term is called with "rho": Quote:
It would be interesting to see if there is any difference in the calculations, comparing the codes or the results from the older version. Regards, Lorenzo |
||
|
|
|
||
|
August 7, 2024, 16:23
|
|
#6 | |
|
Member
Nikos
Join Date: Aug 2012
Location: Greece
Posts: 30
Rep Power: 14 |
Quote:
That was it Lorenzo! Thank you, well appreciated! |
||
|
|
|
||
|
| Tags |
| fvoptions, heat source, scalarcodedsource |
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| [OpenFOAM.org] Patches to compile OpenFOAM 2.2 on Mac OS X | gschaider | OpenFOAM Installation | 136 | October 10, 2017 18:25 |
| polynomial BC | srv537 | OpenFOAM Pre-Processing | 4 | December 3, 2016 10:07 |
| [Other] How to use finite area method in official OpenFOAM 2.2.0? | Detian Liu | OpenFOAM Meshing & Mesh Conversion | 4 | November 3, 2015 04:04 |
| Problem compiling a custom Lagrangian library | brbbhatti | OpenFOAM Programming & Development | 2 | July 7, 2014 12:32 |
| Trouble compiling utilities using source-built OpenFOAM | Artur | OpenFOAM Programming & Development | 14 | October 29, 2013 11:59 |
2Likes
rintStack(Foam::Ostream&)Foam::error :
ptionList:
Linear Mode
