
[Sponsors] 
May 18, 2006, 07:25 
Hi,
I am trying to program a

#1 
Guest
Posts: n/a

Hi,
I am trying to program a radiation model using the Gibb's method (spherical harmonics) I used the "reactingFoam" solver, where I had a file IEqn.H with the following radiation equation : { fvScalarMatrix IEqn ( fvm::laplacian(I)  (I/(4*boltzmannCoeff) + pow(T,4))*(12*pow(knu,2 *boltzmannCoeff) == m ); IEqn.relax(); IEqn.solve(); thermo>correct(); } where I is the radiativ intensity I wanted to get from this equation After the compilation, when I execute reactingFoam, I get this message : > FOAM FATAL ERROR : gradientInternalCoeffs cannot be called for a calculatedFvPatchField. You are probably trying to solve for a field with a calculated or default boundary conditions. From function calculatedFvPatchField<type>::gradientInternalCoef fs() const in file fields/fvPatchFields/basicFvPatchFields/calculated/calculatedFvPatchField.H at line 174. In order to solve the I equation, I need of course some boundary conditions. I though the file I in the "0" directory of the case with the initial and boundary conditions was enough but it is apparently not the case. I try to see in the code an equation file like UEqn.H or hEqn.H but I did not see how the boundary equations are coded Could somebody give me some advices please ? Thank you in advance Julienh 

May 18, 2006, 08:26 
Looks like one of the b.c.s t

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,905
Rep Power: 33 
Looks like one of the b.c.s that you specify in 0/I is not correct or that the field I has been created by calculation rather then read in. Have a look at the place where I is created and pay attention to the MUST_READ and only a mesh argument after the IOobject. For example:
volScalarField I ( IOobject ( "I", runTime.timeName(), mesh, IOobject::MUST_READ, IOobject::AUTO_WRITE ), mesh ); Yours should look exactly the same. Hrv
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

May 18, 2006, 10:13 
Hi,
Thank you for this quick

#3 
Guest
Posts: n/a

Hi,
Thank you for this quick answer. I have exactly the same thing for I in the creatField file. I tried to change the boundary conditions but nothing work, I still have the same error about boundary conditions Best regards julienh 

May 18, 2006, 16:55 
Hi Julien,
it can be a troubl

#4 
Member
Tommaso Lucchini
Join Date: Mar 2009
Posts: 87
Rep Power: 17 
Hi Julien,
it can be a trouble of field definition (or in the createFields or the 0 directory), or a trouble when you try to solve the equation. Could you paste here how is defined I in the 0 directory? And how did you define it in the createFields? What is m? thanks. bye Tommaso 

May 19, 2006, 07:24 
Hi,
I found the mistake, I h

#5 
Guest
Posts: n/a

Hi,
I found the mistake, I had a problem in the calculation of the emissivity, my code works quite well now and calculates the radiativ energy field. I will now try to couple this equation with the basic thermal equation because the convective part of the energy flow emitted by a flame has a direct influence on the radiativ part. But I have difficulties to find where the thermal equation is coded. Does somebody know ? Best regards julienh 

May 23, 2006, 04:28 
Usually hEqn.H

#6 
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 
Usually hEqn.H


June 22, 2006, 06:51 
As you have it coded, I believ

#7 
Senior Member
Michael Prinkey
Join Date: Mar 2009
Location: Pittsburgh PA
Posts: 363
Rep Power: 25 
As you have it coded, I believe the (I/(4*boltzmannCoeff)) term is being treated as an explicit source term and ending up on the RHS. I think what you want to do is use fvm::Sp() to linearize that term and place it on the center coefficient instead. That should improve solution stability.


June 23, 2006, 03:57 
Hello,
Thank you for this

#8 
Guest
Posts: n/a

Hello,
Thank you for this quick answer. I tried to do it with fvm::Sp() but it did not work. But I found one of my mistakes. The maxDeltaT was to large to satisfy the convergence criteria. Now it works but my model uses a fixed value of the optical thickness L and now I want my model to calculate L for each cell with the formula L = (2/3)*(volume of the cell)^(1/3) I coded : volScalarField L = (2/3)*pow (mesh.V(), (1/3)) but it did not work. Could somebody help me please ? Thank you in advance Best regards Julienh 

June 23, 2006, 04:09 
Try
volScalarField L = (2.

#9 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 
Try
volScalarField L = (2.0/3.0)*Foam::pow(mesh.V(), (1.0/3.0)); If you do this a = (1/3) a = 0 Because you are doing integer division. 

June 23, 2006, 08:46 
Thank you very much ! It works

#10 
Guest
Posts: n/a

Thank you very much ! It works like this.
So my very simplified radiation model enables me to calculate the radiation flux I inside my combustion chamber. But to do it, I put boundary conditions for I in the 0 file like fixedValue or zeroGradient. However, the goal of my work is to calculate the field I on the wall of a furnace. The idea is to modify the wallHeatFlux file to add the radiatif flux to the convectif flux. But to do that, instead a BC like zeroGradient for I, I need to put a BC (I0) which is the solution of a new equation : (emissivityWall/4)*I0  boltzmannCoeff*emissivityWall*Twall^4=(1/(3*a))*grad(I(0)) Am I obliged to create a new BC class to do that or is there a other way to do it ? Can somebody give me some advice please ? Thank you in advance Best regards JulienH 

June 27, 2006, 03:36 
Hello,
So, I can calculate th

#11 
Guest
Posts: n/a

Hello,
So, I can calculate the radiation flux within the furnace if I put existing boundary conditions like zeroGradient. But I need to put a calculated value for the boundary condition Iwall of field I. The code calculates Iwall but now I want to put Iwall as a boundary condition for I. So, I think I must code a new BC class. This class must just enable me to fill the /0 field for I like this : internalField uniform 25000; boundayField { walls { type boundaryConditionsforI; value Iwall; } } It is perhaps easy to do that butI am not a very good programmer. Could somebody give me some advise to program my own bounday conditions class please ? Thank you in advance Julien Heintz 

June 28, 2006, 10:16 
Hello,
Finally, I think I do

#12 
Guest
Posts: n/a

Hello,
Finally, I think I do not need to do my own boundary condition class for the field I so I tried to do it differently : here the code I had to my radiation solver in order to calculate the boundary field Iwall : Info<< "\nCreate new boundary condition\n" << endl; label inletPatchID = mesh.boundaryMesh().findPatchID("walls"); fvPatchScalarField& Iwall = I.boundaryField()[inletPatchID]; forAll(Iwall, faceI) { surfaceScalarField Iwall((0.6/epsilonWall)*fvc::snGrad(I) + 4*5.67e8*pow(Tparoi,4)); I.boundaryField()[faceI] = Iwall; } I.write(); Info<< "\n ExecutionTime = " << runTime.elapsedCpuTime() << " s\n" << endl; } but it doesn't work. The field I is calculated but the boundary values of I remain constant, equal to the value I put in the 0/I file. What am I doing wrong ? Thank you in advance julienh 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Radiation P1 Model with Spectral Model: Multigray  A. Thellmann  CFX  0  October 25, 2008 12:44 
Radiation Model  Spectral Model  Ray  CFX  3  April 10, 2006 09:33 
Help: Radiation model  MANOJKUMAR  FLUENT  4  November 24, 2005 02:45 
How to use radiation model with porous model?  jacky  CFX  0  December 17, 2002 22:51 
DO model for RADIATION  Davide  FLUENT  0  October 21, 2001 03:13 