
[Sponsors] 
January 26, 2011, 08:50 
Difference between 'internalField' and 'boundaryField'?

#1 
New Member
Felix W.
Join Date: Jan 2011
Posts: 4
Rep Power: 6 
Dear OFoamers,
as a new user of OpenFoam, I've maybe a very simple question .. but the OFtutorial doesn't give a satisfying answer to me and I become more and more confused (as I tried to make some 'try and error calculations'). What does 'internalField' in e.g. a Ufile describe ? And what is the difference between the 'internalField' and the 'boundaryField' (in detail) ? Thanks in advance, felix 

January 26, 2011, 09:31 

#2 
Senior Member

consider pressure (p), it is defined as volScalarField
means it defines in center of each cell in domain. domain has two parts : domain content (internalField) and domain surrounding (boundaryField). p.boundaryField() give you access to value in boundary, value in boundary would be surface center value. its helpful when you need the maximum, min, sum or average the value of a patch, so it returns a surfaceScalarField. p.internalField() returns a scalarField (im not sure, check it ) , so it can be useful when you want to deal with internal value and keep boundary conditions unchanged. 

January 26, 2011, 09:36 

#3 
New Member
Dominic
Join Date: Jan 2011
Location: Leeds, UK
Posts: 25
Rep Power: 6 
Hi felix,
I'm quite new to OpenFoam myself, but I can give a shot at explaining the internalField condition. For the velocity, U, the internalField characteristic is used to determine the properties of the fluid inside the computational domain. e.g. if the fluid is stationary and there is no velocity in any direction, the value will be uniform (0 0 0), whereas if we are addressing kinetic energy (scalar) and the initial conditions suggest there is some present, the value will be uniform x. In short, as far as I know, (and hopefully right), this condition is simply used to assign the appropriate initial properties to the fluid not located at any of the boundaries. Hope this helps. Dom. 

January 26, 2011, 09:46 

#4 
Senior Member

beside if you just asking about U file in directory 0;
consider you are going to solve a differential equation you need to have boundary condition and initial condition, internalField defines initial condition it can be uniform or nonuniform and boundaryField defines boundary condtion which is mathematical boundary condition likes : fixed value ( means value in that patch is defined ) or zeroGradient ( gradient of the variable in that boundary is zero) look more in user guide 

January 26, 2011, 10:53 

#5 
New Member
Felix W.
Join Date: Jan 2011
Posts: 4
Rep Power: 6 
Hi Nima, hi Dominic,
thanks for your fast replies ! These are exactly my missing information.. Nima: At the moment I'm only looking at some old cases to get known with all the different possibilities for all the settings.. but be sure, that I'll also read further in the user guide ! kind regards, felix 

August 7, 2012, 11:00 

#6  
Senior Member
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6 
Quote:
Thanks for your clear description. Could you please add also that what is the difference between dimensionedInternalField() and InternalField()? I have the following equations. but when I am replacing the dimensionedInternalField() with InternalField() it gives the error. ( and there is no dimensionedboundaryField() ). A.dimensionedInternalField()=min(scalar(0),B.dimen sionedInternalField()); A.boundaryField()=min(scalar(0),B.boundaryField()) ; Best Mahdi 

August 7, 2012, 13:36 

#7 
Senior Member

you know variable has dimension, for example velocity dimension is {m/s}
OpenFOAM saves both variable values and its dimension, so dimensionedInternalField() has besides value of InternalField(), its dimension too! the error returns that you are going to compare a dimensionedvarible with a scalar, it is not allowed, you should define your zero! as a dimensionedScalar with appropriate dimension 

August 7, 2012, 14:51 

#8  
Senior Member
mahdi abdollahzadeh
Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 149
Rep Power: 6 
Quote:
But i was meaning that this formula is ok! Code:
A.dimensionedInternalField()=min(scalar(0),B.dimen sionedInternalField()); Code:
A.InternalField()=min(scalar(0),B.InternalField()); 

April 29, 2014, 12:40 

#10 
Member
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4 
I know this is an old thread but I have a question related to this subject...
I'm trying to write a forAll loop and I keep on getting errors no matter how I code it. I tried coding it this way: Code:
forAll(f1,celli) { if (utau[celli] == 0.0) { f1[celli] = exp(0.5*xn[celli]*utau[celli]/nu()); }else { f1[celli]= 0.0; } } Code:
error: cannot convert ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >’ to ‘double’ in assignment make: *** [Make/linux64GccDPOpt/SPLRRIP.o] Error 1 I understand that f1 is dimensionless, so I have also tried to use .value() instead of [celli] on xn and utau but when I do so, I get the following error: Code:
SPLRRIP.C: In member function ‘virtual void Foam::incompressible::RASModels::SPLRRIP::correct()’: SPLRRIP.C:458:26: error: ‘Foam::volScalarField’ has no member named ‘value’ SPLRRIP.C:458:39: error: ‘Foam::volScalarField’ has no member named ‘value’ make: *** [Make/linux64GccDPOpt/SPLRRIP.o] Error 1 Here is how I have defined utau, f1 and xn. Code:
xn ( IOobject ( "xn", runTime_.timeName(), mesh_, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh_, dimensionedScalar("xn", dimLength, SMALL) ), utau ( IOobject ( "utau", runTime_.timeName(), mesh_, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh_, dimensionedScalar("utau", U_.dimensions(), 0.0) ), f1 ( IOobject ( "f1", runTime_.timeName(), mesh_, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh_, dimensionedScalar("f1", dimless, 0.0) ) xn = wallDist(mesh_).y(); //Normal distance to wall const fvPatchList& Boundaries = mesh_.boundary(); forAll(Boundaries, patchi) //loops through boundaries, patchi is the index { const fvPatch& currPatch = Boundaries[patchi]; //indexed boundary definition (current patch) if (isType<wallFvPatch>(currPatch)) { utauw.boundaryField()[patchi] = sqrt ( nu()*mag(U_.boundaryField()[patchi].snGrad()) ); forAll(currPatch, facei) { label faceCelli = currPatch.faceCells()[facei]; //indexed face in current patch // Assign utau[on indexed cell face] value from utauw[on boundary][at each boundary face] utau[faceCelli] = utauw.boundaryField()[patchi][facei]; forAll(utau, celli) //assigns value of utau[at face] to utau[cells] { utau[celli] = utau[faceCelli]; } } } } 

April 29, 2014, 13:14 

#11 
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
You are dividing by nu(). What is nu()? Is it a field? If so, then you need to access also for nu() the cell values.
In general it's a good idea to get a reference to the internal/boundary fields and loop through these ones. Something like this: Code:
scalarField& f1Cells = f1.internalField(); forAll(f1Cells, cellI) { f1Cells[cellI] = ... } forAll(f1.boundaryField(), patchI) { fvPatchScalarField& pf1 = f1.boundaryField()[patchI]; forAll(pf1, faceI) { pf1[faceI] = ... } } 

April 29, 2014, 13:26 

#12 
Member
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4 
Hello Armin,
I thought nu was the kinematic viscosity defined in constant > transportProperties. Since I'm running incompressible simulations, I assumed that nu() was just a constant value, which is why I wasn't trying to access the individual cell values. However, I tried indexing nu(): Code:
scalarField& f1Cells = f1.internalField(); forAll(f1Cells,celli) { if (utau[celli] == 0.0) { f1Cells[celli] = exp(0.5*xn[celli]*utau[celli]/nu[celli]); }else { f1Cells[celli]= 0.0; } } Code:
SPLRRIP.C:459:58: error: invalid types ‘<unresolved overloaded function type>[Foam::label {aka int}]’ for array subscript make: *** [Make/linux64GccDPOpt/SPLRRIP.o] Error 1 Code:
forAll(f1Cells,celli) { if (utau[celli] == 0.0) { f1Cells[celli] = exp(0.5*xn[celli]*utau[celli]/nu()[celli]); }else { f1Cells[celli]= 0.0; } } Code:
SPLRRIP.C:459:60: error: no match for ‘operator[]’ in ‘Foam::incompressible::turbulenceModel::nu() const()[celli]’ make: *** [Make/linux64GccDPOpt/SPLRRIP.o] Error 1 

April 29, 2014, 13:44 

#13  
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
Quote:
No idea, what goes wrong in your code. Are you sure the error is related to the code you posted initially? Maybe you recheck the line numbers in the error message and source code. 

April 29, 2014, 14:01 

#14 
Member
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4 
Thanks anyway Armin!
I know that the error is caused by the way that I am assigning the value to f1. OpenFOAM doesn't like the f1[celli]=exp(...) The reason (as far as I understand it) is that f1 is a field, but exp(...) returns a double. So, I'm trying to assign a 'double' to a cell within a field. I think I may have figured out a solution to the initial problem... now I have another one Coding it in the following way compiles (I know I should create a label but I'm testing for now): Code:
forAll(f1,celli) { if (utau[celli] == 0.0) { f1.internalField() = exp(0.5*xn[celli]*utau[celli]/nu()); }else { f1.internalField()= scalar(0.0); } } Code:
Starting time loop Time = 1e05 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.36617e07, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.36614e07, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.999805, Final residual = 9.67079e07, No Iterations 531 time step continuity errors : sum local = 3.21009e14, global = 1.1476e17, cumulative = 1.1476e17 [0] [0] [0] > FOAM FATAL ERROR: [0] Argument of trancendental function not dimensionless [0] [0] From function trans(const dimensionSet&) [0] in file dimensionSet/dimensionSet.C at line 424. [0] FOAM parallel run aborting [0] 

April 29, 2014, 14:20 

#15  
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
Quote:
f1 may be a field, but you can very well assign 'double' values to a cell. In fact when you do Code:
f1Cells[cellI] = 3.141592; Well, the solution for you is to bisect your code. Meaning, start with assigning 'double' values (e.g. 3.141592) to your cells and see if it compiles. If that works, add step by step more functions and see where it starts to go wrong. Good luck! 

April 29, 2014, 14:25 

#16  
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
Quote:
Where is that code anyways? In a solver or a library? Maybe you try to switch back to my initial example with the reference to the internal field and remove the nu(). Does that compile? 

April 29, 2014, 16:01 

#17 
Member
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4 
Armin,
The code is part of a turbulence model (LRR). I tried doing Code:
f1Cells[cellI]=3.141564 I removed nu() and substituted it with it's numerical value and it compiled and ran! So the whole problem was being caused by nu(). How would you access the value of nu so that the loop will adopt the numerical value for the current simulation? The reason why I am confused is that I am able to access nu whenever it is outside of a loop. For example, if I have Code:
f1=exp(0.5*xn*utau/nu()); The problem arises when nu() is used in the loop... 

April 30, 2014, 05:52 

#18  
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
Quote:
Look up the return type of nu() and you will have the solution to your problem. Random testing will just waist your time here. My guess is that it is a tmpfield... 

April 30, 2014, 12:59 

#19 
Member
CHARLES
Join Date: May 2013
Posts: 46
Rep Power: 4 
That is a great question... After looking in transportModels/incompressible/viscosityModels/Newtonian I have learned that nu() is in fact a tmp field:
Code:
// Member Functions // Return the laminar viscosity tmp<volScalarField> nu() const { return nu_; } I don't understand why nu() can be accessed in a nonloop way but not from within a loop. Thank you so much for taking the time to work through this with me. 

May 2, 2014, 06:07 

#20  
Senior Member
Armin
Join Date: Feb 2011
Location: Helsinki, Finland
Posts: 152
Rep Power: 10 
Quote:
http://openfoamwiki.net/index.php/OpenFOAM_guide/tmp tmp  stands for 'true macro pain'? A fix to your problem would be something like this: Code:
const scalarField& nuCells = nu()().internalField(); Code:
f1Cells[cellI] = 3.141564*nuCells[cellI]; 

Tags 
boundaryfield, internalfield 
Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
boundary conditions for simpleFoam calculation  foam_noob  OpenFOAM Running, Solving & CFD  8  July 1, 2015 08:07 
boundaryField vs. internalField  sebonator  OpenFOAM  10  January 24, 2011 17:43 
solidWallHeatFluxTemperature at the solid solid interface in chtMultiRegionSimpleFoam  maddalena  OpenFOAM Running, Solving & CFD  43  January 11, 2011 03:39 
buoyantSimpleRadiationFoam  msarkar  OpenFOAM  0  February 15, 2010 07:22 
pipe flow with heat transfer  Fabian  OpenFOAM  2  December 12, 2009 05:53 