# New boundary condition

 Register Blogs Members List Search Today's Posts Mark Forums Read

 April 14, 2009, 06:03 #21 New Member   L.E.Tonkov Join Date: Apr 2009 Posts: 3 Rep Power: 8 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, 21:19
#22
Senior Member

ZHOU Bin
Join Date: Mar 2009
Location: Nanjing/Shanghai/Torino, Nanjing/Shanghai/Piemente, China/Italy
Posts: 164
Rep Power: 8
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

Quote:
 Originally Posted by niklas Hola, Not 100 percent sure, but I'd say its like this: valueFraction*U + (1-valueFraction)*dU = 0 N

 June 9, 2009, 02:49 #23 Senior Member   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 213 Rep Power: 10 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 "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben Franz-Josef-Str. 18 A - 8700 Leoben Österreich / Austria Tel.: +43 3842 - 402 - 3125 http://smmp.unileoben.ac.at

 June 24, 2010, 15:09 #24 Member   Dinesh Nath Join Date: Dec 2009 Location: Kanpur, India Posts: 39 Rep Power: 7 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 dinesh2n@gmail.com; June 25, 2010 at 01:22.

 October 6, 2010, 00:46 #25 Member   Join Date: Dec 2009 Posts: 46 Rep Power: 7 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 16:44.

October 6, 2010, 16:48
#26
Member

Join Date: Dec 2009
Posts: 46
Rep Power: 7
Quote:
 Originally Posted by zhoubinwx 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
That is a good post

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, 02:31 #27 Senior Member   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 213 Rep Power: 10 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 00143 void mixedFvPatchField::evaluate(const Pstream::commsTypes) 00144 { 00145 if (!this->updated()) 00146 { 00147 this->updateCoeffs(); 00148 } 00149 00150 Field::operator= 00151 ( 00152 valueFraction_*refValue_ 00153 + 00154 (1.0 - valueFraction_)* 00155 ( 00156 this->patchInternalField() 00157 + refGrad_/this->patch().deltaCoeffs() 00158 ) 00159 ); 00160 00161 fvPatchField::evaluate(); 00162 } 00163 00164 00165 template 00166 tmp > mixedFvPatchField::snGrad() const 00167 { 00168 return 00169 valueFraction_ 00170 *(refValue_ - this->patchInternalField()) 00171 *this->patch().deltaCoeffs() 00172 + (1.0 - valueFraction_)*refGrad_; 00173 }``` That mean, 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 "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben Franz-Josef-Str. 18 A - 8700 Leoben Österreich / Austria Tel.: +43 3842 - 402 - 3125 http://smmp.unileoben.ac.at

February 17, 2011, 11:15
#28
New Member

Raimonds Vilums
Join Date: Oct 2010
Posts: 17
Rep Power: 7
To implement something like this
Quote:
 Originally Posted by makaveli_lcf T - T_ext - k_f /h_f * d(T)/dn = 0 (3)
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))";
}```
For explanation, see thread Mixed BC - heat transfer - laplacianFoam

 February 8, 2012, 14:31 Partial slip boundary #29 Senior Member   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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 >::constructpatchConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0xcc): undefined reference to `Foam::fvPatchField >:atchConstructorTablePtr_' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0xef): undefined reference to `Foam::fvPatchField >::constructpatchMapperConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x10f): undefined reference to `Foam::fvPatchField >:atchMapperConstructorTablePtr_' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x132): undefined reference to `Foam::fvPatchField >::constructdictionaryConstructorTables()' particleSlipJohnsonJacksonFvPatchVectorField.C.t ext.startup+0x152): undefined reference to `Foam::fvPatchField >::dictionaryConstructorTablePtr_' collect2: ld returned 1 exit status someone can help me? Thanks in advance

 February 27, 2012, 17:34 particleSlipJohnsonJackson #31 Senior Member   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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(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::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 >::evaluate(Foam::UPstream::commsTypes) in "/opt/openfoam201/platforms/linuxGccDPOpt/lib/libfiniteVolume.so" #5 Foam:articleSlipJohnsonJacksonFvPatchVectorField:a rticleSlipJohnsonJacksonFvPatchVectorField(Foam::f vPatch const&, Foam:imensionedField, Foam::volMesh> const&, Foam::dictionary const&) in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libJohnsonJackson.so" #6 Foam::fvPatchField >::adddictionaryConstructorToTable::New(Foam::fv Patch const&, Foam:imensionedField, Foam::volMesh> const&, Foam::dictionary const&) in "/home/recepkati/OpenFOAM/recepkati-2.0.1/platforms/linuxGccDPOpt/lib/libJohnsonJackson.so" #7 Foam::fvPatchField >::New(Foam::fvPatch const&, Foam:imensionedField, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #8 Foam::GeometricField, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::GeometricB oundaryField(Foam::fvBoundaryMesh const&, Foam:imensionedField, Foam::volMesh> const&, Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #9 Foam::GeometricField, Foam::fvPatchField, Foam::volMesh>::readField(Foam::dictionary const&) in "/opt/openfoam201/platforms/linuxGccDPOpt/bin/twoPhaseEulerFoam" #10 Foam::GeometricField, 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

Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
Quote:
 request for dictionary kineticTheoryProperties from objectRegistry region0 failed available objects of type dictionary are
You need that dictionary for your solver.
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at

 February 28, 2012, 06:22 particleSlipJohnsonJackson #33 Senior Member   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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

Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
Quote:
 and I have the directory kineticTheoryProperties in the model.
That should be a file in "constant/" folder, see
bed2/constant/kineticTheoryProperties

in tutorial
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at

February 28, 2012, 06:33
particleSlipJohnsonJackson
#35
Senior Member

rkhr
Join Date: May 2011
Posts: 209
Rep Power: 7
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
Attached Files
 particleSlipJohnsonJacksonFvPatchVectorField.C (5.8 KB, 24 views)

 February 28, 2012, 07:46 #36 Senior Member   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 213 Rep Power: 10 Do you have this file in your case folder? __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben Franz-Josef-Str. 18 A - 8700 Leoben Österreich / Austria Tel.: +43 3842 - 402 - 3125 http://smmp.unileoben.ac.at

February 28, 2012, 07:48
#37
Senior Member

Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
Ok, if you look in your BC file

Quote:
 void particleSlipJohnsonJacksonFvPatchVectorField::upda teCoeffs() { if (updated()) { return; } if ((specularityCoefficient_ < 0) || (specularityCoefficient_ > 1)) { FatalErrorIn ( "particleSlipJohnsonJacksonFvPatchScalarField: :" "updateCoeffs()" ) << "The value of the specularity coefficient has to be between 0 and 1." << abort(FatalError); } const dictionary& transportProperties = db().lookupObject ( "transportProperties" ); const dictionary& kineticTheoryProperties = db().lookupObject ( "kineticTheoryProperties" ); ...
so your BC looks for the dictionary kineticTheoryProperties in the memory,
but does not find.

Which solver do you use?
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at

 February 28, 2012, 07:49 particleSlipJohnsonJackson #38 Senior Member   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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   Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 213 Rep Power: 10 no, that which you send me __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben Franz-Josef-Str. 18 A - 8700 Leoben Österreich / Austria Tel.: +43 3842 - 402 - 3125 http://smmp.unileoben.ac.at

 February 28, 2012, 07:52 particleSlipJohnsonJackson #40 Senior Member   rkhr Join Date: May 2011 Posts: 209 Rep Power: 7 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Tomik FLUENT 0 December 5, 2006 18:37 plage OpenFOAM Running, Solving & CFD 4 October 3, 2006 12:21 Shukla Main CFD Forum 3 November 11, 2005 16:02 Jeff FLUENT 2 November 20, 2003 18:15 Zhang Tsiang Main CFD Forum 3 February 5, 2002 21:15

All times are GMT -4. The time now is 17:46.