|
[Sponsors] |
April 14, 2009, 07:03 |
|
#21 |
New Member
L.E.Tonkov
Join Date: Apr 2009
Posts: 3
Rep Power: 17 |
Thank you, Alexander for fast reply. As far as I understand inletOutlet, b.c. depend on U vector direction but not magnitude.
I send forum private message to you. Best regards Leonid |
|
June 8, 2009, 22:19 |
|
#22 |
Senior Member
|
Hello,
Can I ask in " valueFraction*U + (1-valueFraction)*dU = 0 ", dU means the normal gradient of U, i.e. dU/dn, or just the difference between internalField velocity and boundary velocity? Bin |
|
June 9, 2009, 03:49 |
|
#23 |
Senior Member
|
According to User Guide page 128 it is normal gradient. Learn to use documentation for such questions, it will be more usefull:-)
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
|
June 24, 2010, 16:09 |
|
#24 |
Member
Join Date: Dec 2009
Location: Kanpur, India
Posts: 54
Rep Power: 16 |
Hello makaveli_lcf
You wrote that you had written your own code for dT/dn = h_ext / k_f * (T_ext - T) this kind of BC. I am trying to solve a problem which concerns the same BC you have talked in post #18. Could you please send me your code of that BC. I would be grateful to you. thanks Last edited by Shoonya; June 25, 2010 at 02:22. |
|
October 6, 2010, 01:46 |
|
#25 |
Member
Join Date: Dec 2009
Posts: 46
Rep Power: 16 |
Hi,
the equation valueFraction * U + (1 - valueFraction) * dU/dy = 0 is not dimensionally consistent !! i think it should be valueFraction * U + (1 - valueFraction) *dU= 0 which dU is only the velocity difference any comments ? thanks Last edited by openfoam1; October 6, 2010 at 17:44. |
|
October 6, 2010, 17:48 |
|
#26 | |
Member
Join Date: Dec 2009
Posts: 46
Rep Power: 16 |
Quote:
dU is not dU/dn it is just the difference between internalField velocity and boundary velocity because the equation must be dimensionally consistent by the way , i verified it using simple mesh and icoFoam solver thank you |
||
October 7, 2010, 03:31 |
|
#27 |
Senior Member
|
It is not necessary to guess what is what. Just have a look at the source code, otherwise why do we need it)))
So, from mixedFvPatchField.C: Code:
00142 template<class Type> 00143 void mixedFvPatchField<Type>::evaluate(const Pstream::commsTypes) 00144 { 00145 if (!this->updated()) 00146 { 00147 this->updateCoeffs(); 00148 } 00149 00150 Field<Type>::operator= 00151 ( 00152 valueFraction_*refValue_ 00153 + 00154 (1.0 - valueFraction_)* 00155 ( 00156 this->patchInternalField() 00157 + refGrad_/this->patch().deltaCoeffs() 00158 ) 00159 ); 00160 00161 fvPatchField<Type>::evaluate(); 00162 } 00163 00164 00165 template<class Type> 00166 tmp<Field<Type> > mixedFvPatchField<Type>::snGrad() const 00167 { 00168 return 00169 valueFraction_ 00170 *(refValue_ - this->patchInternalField()) 00171 *this->patch().deltaCoeffs() 00172 + (1.0 - valueFraction_)*refGrad_; 00173 } U_wall = valueFraction*U0 + (1 - valueFraction)*(U_nearwall + Grad0 * dn) where U0 and Grad0 are our given reference values for boundary field and gradient at the wall. dn is the distance between center of the cell and the boundary face. Now it is possible to transform this condition in whatever form is necessary))) All gradients and matrix coefficients are calculated using this relation. Good luck!
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
|
February 17, 2011, 11:15 |
|
#28 |
New Member
Raimonds Vilums
Join Date: Oct 2010
Posts: 17
Rep Power: 17 |
To implement something like this
you could use groovyBC from swak4foam in the similar manner like the following code: Code:
rightWall { type groovyBC; variables "h_f=20.0;T_ext=20.0;k_f=0.2;"; valueExpression "T_ext"; fractionExpression "1.0/(1.0 + k_f/(mag(delta())*h_f))"; } |
|
February 8, 2012, 14:31 |
Partial slip boundary
|
#29 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
thank u in advance!
Last edited by Kanarya; February 17, 2012 at 12:29. |
|
February 17, 2012, 12:26 |
ParticalSlip in OpenFOAM210
|
#30 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
hi Foamers,
I am trying to compile particleSlip BC but it gives me error. can it be because of the version of OpenFoam because Alberto did code 2009 or 2010?can be the headers are different? The error is: Make/linux64GccDPOpt/particleSlipJohnsonJacksonFvPatchVectorField.o: In function `_GLOBAL__sub_I_particleSlipJohnsonJacksonFvPatchV ectorField.C': particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0xaf): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructpatchConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0xcc): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >:atchConstructorTablePtr_' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0xef): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructpatchMapperConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x10f): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >:atchMapperConstructorTablePtr_' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x132): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::constructdictionaryConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x152): undefined reference to `Foam::fvPatchField<Foam::Vector<double> >::dictionaryConstructorTablePtr_' collect2: ld returned 1 exit status someone can help me? Thanks in advance |
|
February 27, 2012, 17:34 |
particleSlipJohnsonJackson
|
#31 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
Hi Foamers,
I would like to apply particleSlip BCs but I have following error and I could not find out the problem...please help me.. Create mesh for time = 0 Reading g Reading transportProperties --> FOAM FATAL ERROR: request for dictionary kineticTheoryProperties from objectRegistry region0 failed available objects of type dictionary are 4 ( fvSchemes fvSolution data transportProperties ) From function objectRegistry::lookupObject<Type>(const word&) const in file /opt/openfoam201/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 131. FOAM aborting #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/libOpenFOAM.so" #2 Foam::IOdictionary const& Foam:bjectRegistry::lookupObject<Foam::IOdiction ary>(Foam::word const&) const in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #3 Foam:articleSlipJohnsonJacksonFvPatchVectorField ::updateCoeffs() in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libJohnsonJackson.so" #4 Foam:artialSlipFvPatchField<Foam::Vector<double> >::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #5 Foam:articleSlipJohnsonJacksonFvPatchVectorField:a rticleSlipJohnsonJacksonFvPatchVectorField(Foam::f vPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libJohnsonJackson.so" #6 Foam::fvPatchField<Foam::Vector<double> >::adddictionaryConstructorToTable<Foam:articleS lipJohnsonJacksonFvPatchVectorField>::New(Foam::fv Patch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libJohnsonJackson.so" #7 Foam::fvPatchField<Foam::Vector<double> >::New(Foam::fvPatch const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #8 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricB oundaryField(Foam::fvBoundaryMesh const&, Foam:imensionedField<Foam::Vector<double>, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #9 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #10 Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh>::readField(Foam::Istream&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #11 at phaseModel.C:0 #12 Foam:haseModel:haseModel(Foam::fvMesh const&, Foam::dictionary const&, Foam::word const&) in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libphaseModel.so" Aborted thanks in advance.. |
|
February 28, 2012, 03:46 |
|
#32 | |
Senior Member
|
Quote:
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
||
February 28, 2012, 06:22 |
particleSlipJohnsonJackson
|
#33 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
Hi Alex,
thank you very much for your quick answer. I have already the directory there. I am using twoPhaseEulerFoam solver and I implement particleSlipJohnsonJackson BC in the model which is also from tutorials case "bed2".my file looks like: dimensions [0 1 -1 0 0 0 0]; internalField uniform (0 0 0); boundaryField { walls { type particleSlipJohnsonJackson; specularityCoefficient 0.5; } outlet { type zeroGradient; } inlet { type fixedValue; value uniform (0 0 0); } frontAndBackPlanes { type empty; } } I changed BC of the walls. and I have the directory kineticTheoryProperties in the model. thanks a lot again |
|
February 28, 2012, 06:25 |
|
#34 | |
Senior Member
|
Quote:
bed2/constant/kineticTheoryProperties in tutorial
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
||
February 28, 2012, 06:33 |
particleSlipJohnsonJackson
|
#35 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
Hi Alex,
yes I had a look to this file but I could not find the problem what I should add there? I attached the code as well. thank you very much and I appreciate your time to send me this suggestions. recep |
|
February 28, 2012, 07:46 |
|
#36 |
Senior Member
|
Do you have this file in your case folder?
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
|
February 28, 2012, 07:48 |
|
#37 | |
Senior Member
|
Ok, if you look in your BC file
Quote:
but does not find. Which solver do you use?
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
||
February 28, 2012, 07:49 |
particleSlipJohnsonJackson
|
#38 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
hi Alex,
I think you forget to say the name of the file, which file? best regards and thanks again recep |
|
February 28, 2012, 07:50 |
|
#39 |
Senior Member
|
no, that which you send me
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at |
|
February 28, 2012, 07:52 |
particleSlipJohnsonJackson
|
#40 |
Senior Member
Join Date: May 2011
Posts: 231
Rep Power: 16 |
hi Alex
I am using twoPhaseEulerFoam. yes, I understood the problem but I do not know how to modify it. thanks Recep |
|
Tags |
heat transfer, new bc |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Boundary condition for UDS | Tomik | FLUENT | 0 | December 5, 2006 18:37 |
Boundary condition of the third kind or Danckwertz boundary condition | plage | OpenFOAM Running, Solving & CFD | 4 | October 3, 2006 13:21 |
Slip Boundary Condition for Moving Boundary | Shukla | Main CFD Forum | 3 | November 11, 2005 16:02 |
UDF boundary condition | Jeff | FLUENT | 2 | November 20, 2003 18:15 |
Boundary Condition in LES | Zhang Tsiang | Main CFD Forum | 3 | February 5, 2002 21:15 |