|
[Sponsors] |
June 30, 2010, 10:53 |
Implementation of a new volField
|
#1 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Dear all,
I'm trying to implement a new volField of a new type of VectorField, for example a vector of n elements. This is my workplan: first of all I should define a new template class of my new type, copying from Vector.H Code:
class Vector : public VectorSpace<Vector<Cmpt>, Cmpt, 3> Then adapting from VectorI.H I define the operations I need. Next I typedef for scalar (for example) version of the new templated n-Vector, copying from vector.H. Included here there is contiguous.H, can somebody explain what it does, please? Now I have a primitive type, and I can instantiate a Field, as Code:
typedef GeometricField<nVector, fvPatchField, volMesh> volNVectorField; Hope somebody can help me, best regards Andrea |
|
July 2, 2010, 05:37 |
error, undefined reference to ...
|
#2 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Ok, when I construct a volNVectorField as usual
Code:
volNVectorField myVolNVectorField ( IOobject ( "goofy", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh ); Code:
undefined reference to `Foam::calculatedFvPatchField<Foam::NVector<double> >::typeName' Make/linuxGccDPOpt/mySolver.o: In function `Foam::fvPatchField<Foam::NVector<double> >::type() const': mySolver.C:(.text._ZNK4Foam12fvPatchFieldINS_7NVectorIdEEE4typeEv[Foam::fvPatchField<Foam::NVector<double> >::type() const]+0x11): undefined reference to `Foam::fvPatchField<Foam::NVector<double> >::typeName'' Best regards Andrea |
|
July 2, 2010, 09:09 |
|
#3 |
Senior Member
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 403
Rep Power: 25 |
You're probably getting the error because the default patch type for a GeometricField is the calculated type. During template instantiation, the compiler looks for a calculated patchField type which (in your case) should be a templated patchField for 'nVector'.
Take a look at the makeFvPatchField() macros, and that should give you some direction. It does seem a little odd that you would want to customize a vectorSpace definition - do the current ones not fit your needs? |
|
July 5, 2010, 12:44 |
It compiles but solver crashes
|
#4 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Hi,
thanks deepsterblue, yes the vector spaces already defined in OF are barely all we need. But in my calculation I need to store a n number of data on the patch surface that are function of other fields, I would like to access these data and manipulate them as an ordinary volField (read and write them for example). I thought that a volNVectorField could fit my needs. If anybody as a clever idea, please share. Now I'm able to define a nvector now, plus a volNVectorField as Code:
volNVectorField myNVectorField ( IOobject ( "myNVectorField", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), mesh, dimensionSet(0,0,0,0,0,0,0), "fixedValue" ); Code:
#0 Foam::error::printStack(Foam::Ostream&) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::fvPatchField<Foam::NVector<double> >::New(Foam::word const&, Foam::fvPatch const&, Foam::DimensionedField<Foam::NVector<double>, Foam::volMesh> const&) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver" #4 Foam::GeometricField<Foam::NVector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricBoundaryField(Foam::fvBoundaryMesh const&, Foam::DimensionedField<Foam::NVector<double>, Foam::volMesh> const&, Foam::word const&) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver" #5 Foam::GeometricField<Foam::NVector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricField(Foam::IOobject const&, Foam::fvMesh const&, Foam::dimensionSet const&, Foam::word const&) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver" #6 main in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver" #7 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #8 _start in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver.C" Segmentation fault Andrea |
|
July 6, 2010, 10:38 |
|
#5 |
Senior Member
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 403
Rep Power: 25 |
Not a very useful stack trace... Compile your libraries in debug, and set FOAM_ABORT to true. This should give you the exact line where the seg-fault occurs..
|
|
July 7, 2010, 10:18 |
Some improvements but stopped again
|
#6 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Thanks for the hint,
I added these lines to my solver Code:
typedef fvPatchField<nvector> fvPatchNVectorField; makeFvPatchField(fvPatchNVectorField) typedef calculatedFvPatchField<nvector> calculatedFvPatchNVectorField; defineTemplateTypeNameAndDebug(calculatedFvPatchNVectorField, 0); typedef DimensionedField<nvector, volMesh> DimensionedNVectorField; typedef GeometricField<nvector, fvPatchField, volMesh> volNVectorField; defineTemplateTypeNameAndDebug(volNVectorField::DimensionedInternalField, 0); defineTemplateTypeNameAndDebug(volNVectorField, 0); Code:
DimensionedNVectorField myDimNVectorField( IOobject ( "myDimNVectorField", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), mesh, dimensionSet(0,0,1,0,0,0,0) ); If I leave the default "calculated", the debug mode gives me a printStack Code:
#0 Foam::error::printStack(Foam::Ostream&) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigSegv::sigSegvHandler(int) in "/home/andrea/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::HashTable<Foam::tmp<Foam::fvPatchField<Foam::NVector<double> > > (*)(Foam::fvPatch const&, Foam::DimensionedField<Foam::NVector<double>,Foam::volMesh> const&), Foam::word, Foam::string::hash>::find(Foam::word const&) at ~/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/HashTable.C:177 #4 Foam::fvPatchField<Foam::NVector<double> >::New(Foam::word const&, Foam::fvPatch const&, Foam::DimensionedField<Foam::NVector<double>, Foam::volMesh> const&) at ~/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/newFvPatchField.C:46 #5 GeometricBoundaryField at ~/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricBoundaryField.C:56 #6 GeometricField at ~/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/GeometricField.C:201 #7 main at ~/OpenFOAM/andrea-1.6/Myapplications/solvers/mySolver/AndreaMassFlowBC/mySolver.C:97 #8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #9 _start in "/home/andrea/OpenFOAM/OpenFOAM-1.6/applications/bin/linuxGccDPOpt/mySolver" Segmentation fault Code:
// GeometricField.C:201 boundaryField_(mesh.boundary(), *this, patchFieldType) { if (debug) // error { Info<< "GeometricField<Type, PatchField, GeoMesh>::GeometricField : " "creating temporary" << endl << this->info() << endl; } readIfPresent(); } // GeometricBoundaryField.C 56 forAll(bmesh_, patchi) { set // error ( patchi, PatchField<Type>::New ( patchFieldType, bmesh_[patchi], field ) ); // newFvPatchField.C:46 typename patchConstructorTable::iterator cstrIter = patchConstructorTablePtr_->find(patchFieldType); // error // HashTable.C:177 if (nElmts_) // error { const label hashIdx = hashKeyIndex(key); for (hashedEntry* ep = table_[hashIdx]; ep; ep = ep->next_) { if (key == ep->key_) { return iterator(*this, ep, hashIdx); } } } Andrea |
|
July 7, 2010, 11:30 |
|
#7 |
Senior Member
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 403
Rep Power: 25 |
You might want to check whether the calculated type is added to the run-time selection tables during the run. If I'm not mistaken, initializing the volField with a wrong patchField type (like bananaFvPatchNVectorField, for instance :P) should give you the list of possible types.
|
|
July 8, 2010, 12:03 |
|
#8 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Thanks again,
I really appreciate your help. I've checked, I initiated the volField to be MUST_READ than I try different type in the first boundaryField patch. For any type of patch, banana, fixedValue and even if I leave it blank as "patchName {type ; }", I get the same error message. If I drop also "type" it complains about that is missing. I'm running out of ideas but for the following: what would you think of implementing the same stuff into the OF libraries? This sounds as a sort of last call to me... Andrea Last edited by andrea; July 9, 2010 at 06:16. |
|
July 9, 2010, 06:17 |
|
#9 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Let's cross fingers, knock on wood etc.
maybe I found a way out, stay tuned! Andrea |
|
July 9, 2010, 09:45 |
calculatedFvPatchNVectorField ok but...
|
#10 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Hi,
good new first. Adding these lines Code:
typedef calculatedFvPatchField<nvector> calculatedFvPatchNVectorField; makePatchTypeField ( fvPatchNVectorField, calculatedFvPatchNVectorField ); Bad new now. At the moment I get only one patchField Type available Code:
Unknown patchField type fixedValue for patch type patch Valid patchField types are : 1 ( calculated ) Code:
/home/andrea/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/fixedValueFvPatchField.C: In member function ‘Foam::tmp<Foam::Field<Type> > Foam::fixedValueFvPatchField<Type>::gradientInternalCoeffs() const [with Type = Foam::NVector<double>]’: andreaMassFlowBC.C:293: instantiated from here /home/andrea/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:121: error: conversion from ‘Foam::tmp<Foam::Field<Foam::Vector<double> > >’ to non-scalar type ‘Foam::tmp<Foam::Field<Foam::NVector<double> > >’ requested /home/andrea/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/FieldFunctions.C: In function ‘void Foam::outer(Foam::Field<typename Foam::outerProduct<Form, Type>::type>&, const Foam::VectorSpace<Form, Cmpt, nCmpt>&, const Foam::UList<Type>&) [with Form = Foam::NVector<double>, Cmpt = double, int nCmpt = 10, Type = double]’: /home/andrea/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/FieldFunctions.C:693: instantiated from ‘Foam::tmp<Foam::Field<typename Foam::outerProduct<Form, Type>::type> > Foam::operator*(const Foam::VectorSpace<Form, Cmpt, nCmpt>&, const Foam::UList<Type>&) [with Form = Foam::NVector<double>, Cmpt = double, int nCmpt = 10, Type = double]’ /home/andrea/OpenFOAM/OpenFOAM-1.6/src/finiteVolume/lnInclude/fixedValueFvPatchField.C:121: instantiated from ‘Foam::tmp<Foam::Field<Type> > Foam::fixedValueFvPatchField<Type>::gradientInternalCoeffs() const [with Type = Foam::NVector<double>]’ andreaMassFlowBC.C:293: instantiated from here /home/andrea/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/FieldFunctions.C:693: error: no match for ‘operator=’ in ‘*(Foam::outer(Foam::Field<typename Foam::outerProduct<Form, Type>::type>&, const Foam::VectorSpace<Form, Cmpt, nCmpt>&, const Foam::UList<Type>&) [with Form = Foam::NVector<double>, Cmpt = double, int nCmpt = 10, Type = double]::productType*)(f1P ++) = Foam::operator*(const Foam::VectorSpace<Form, Cmpt, nCmpt>&, Foam::scalar) [with Form = Foam::NVector<double>, Cmpt = double, int nCmpt = 10]((*(const double*)(f2P ++)))’ /home/andrea/OpenFOAM/OpenFOAM-1.6/src/OpenFOAM/lnInclude/Vector.H:62: note: candidates are: Foam::Vector<double>& Foam::Vector<double>::operator=(const Foam::Vector<double>&) make: *** [Make/linuxGccDPOpt/andreaMassFlowBC.o] Error 1 But, since I don't need to add this volNVectorField to any fvMatrix should I better re-implement a fixedValueNVecor patch re-defining - valueInternalCoeffs - valueBoundaryCoeffs - gradientInternalCoeffs - gradientBoundaryCoeffs ? I just need a calculated type, and a type that let me to modify runtime through updateCoeffs() the values of my volField, maybe can I derive it from calculated, is it a good idea? Andrea Last edited by andrea; July 9, 2010 at 10:15. |
|
July 12, 2010, 18:18 |
|
#11 |
Senior Member
Sandeep Menon
Join Date: Mar 2009
Location: Amherst, MA
Posts: 403
Rep Power: 25 |
Looks like you're running into vector-space issues involving tensorial products. Why use updateCoeffs to update boundary patch values? Couldn't you just use (pseudocode):
field.boundaryField()[patch] = Field<nVector>(patch.size()); I think a calculated type should be just fine, particularly if you're not looking to solve anything on it. |
|
July 14, 2010, 11:26 |
succeed
|
#12 |
Member
Andrea Petronio
Join Date: Mar 2009
Location: Trieste, Italy
Posts: 43
Rep Power: 17 |
Ok,
my last post on this just to thanks Deepsterblue for the precious help. I succeed in developing also a boundary condition-like (it does not update any coefficients) but implementing the code I need in the updateCoeffs() I take advantage of all the OF machinery in order to manage data. Bye Andrea |
|
Tags |
geometricfield, primitive type, vectorspace, volfield |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
OpenFOAM141dev A new implementation of dynamicKistlerGammaContactAngle | eberberovic | OpenFOAM Running, Solving & CFD | 26 | June 10, 2021 05:08 |
Problems with own LES Model Implementation | fs82 | OpenFOAM | 1 | October 9, 2009 11:31 |
Please explain the implementation of species transport Eqn in reactingFoam | kallipygian | OpenFOAM Running, Solving & CFD | 0 | October 13, 2008 08:29 |
FEM Implementation of pressure-correction scheme | Markus | Main CFD Forum | 4 | January 6, 2007 02:53 |
Implementation of wall function with SA model | Bala | Main CFD Forum | 0 | October 8, 2004 00:54 |