
[Sponsors] 
July 9, 2009, 21:34 
how to program the formula ddy(ux)+ddx(uy)

#1 
New Member
yan
Join Date: Mar 2009
Posts: 2
Rep Power: 0 
hi, foamers. i want to implement the formula ddy(ux)+ddx(uy) in program, can you tell how to write in source code? thanks


July 10, 2009, 20:20 

#2 
Senior Member

you can try
volScalarField ux=u.component(0); volScalarField uy=u.component(1); volVectorField gradux=fvc::grad(ux); volVectorField graduy=fvc::grad(uy); your formulation: gradux.component(1)+graduy.component(0); or volTensorField gradU=fvc::grad(U) volSymmTensorField twoSymmGradu=twoSymm(gradU); your formulation is twoSymmGradu.component(1); Junwei Last edited by su_junwei; July 11, 2009 at 08:27. 

July 15, 2009, 05:00 

#3 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
And do you know how to program this?
x / (x² + y²) 

July 15, 2009, 05:49 

#4 
Senior Member

const volVectorField & C=mesh.C();
volScalarField x=C.component(0); volScalarField y=C.component(1); your formulation x/(sqr(x)+sqr(y)) Junwei 

July 15, 2009, 06:18 

#5 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 277
Rep Power: 11 
or even simpler, if z is zero:
Code:
const volVectorField & C=mesh.C(); volScalarField res = C.component(vector::X)/magSqr(C); 

July 24, 2009, 11:09 

#6 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
Thank you very much. Sorry for disturb you again, but I have other problem:
I need a function_new which values x/(x² + ²) if x > 0 and 1 if x < 0 So I have tipped const volVectorField & C = mesh.C(); volScalarField x = C.component(0); volScalarField y = C.component(1); volScalarField function = x/(sqrt(x)+sqrt(y)); volScalarField function_new = scalar(1); forAll(x, gI) { if (x[gI] < 0) function_new[gI] = 1; else function_new[gI] = function[gI]; } I have no errors but “fuction_new” always is “1”. I think that the error is that “gI” is not the word I have to type. 

July 24, 2009, 12:30 

#7 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 277
Rep Power: 11 
Isabel,
the long answer is: I do not see what's wrong. Try and put some Infostatements into the loop and ifstatement. the short answer is: Code:
volScalarField function_new = max(function, scalar(0)); Henrik 

July 24, 2009, 13:04 

#8 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
Thank you very much, Henrik. But my error continues. To see the error better, I have tipped this:
volScalarField x = C.component(0); volScalarField function_new = scalar(1); forAll(x,gI) { function_new[gI] = x[gI]; } And when I execute, “function_new” always is 1 and should be equal to "x" Why is always 1? 

July 24, 2009, 13:26 

#9 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
Sorry Henrik, you were right. I have discovered that I was other different problem. These lines were Ok.
Only a last doubt, I don't know which is better: use forAll(x,gI) or forAll(x,celli) ??? 

July 24, 2009, 14:06 

#10 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 277
Rep Power: 11 
Isabel,
the difference between the two statements is only the name of the variable  Nothing else. Henrik 

August 19, 2009, 10:50 

#11 
New Member
Benjamin
Join Date: May 2009
Posts: 5
Rep Power: 10 
Hi,
why is it not possible to do: volVectorField Grad_X volTensorField gradU=fvc::grad(U); Info << gradU.T()*Grad_X << endl ; It gaves me the following error: no match for ‘operator*’ in ‘Foam::GeometricField<Type, PatchField, GeoMesh>::T() const [with Type = Foam::Tensor<double>, PatchField = Foam::fvPatchField, GeoMesh = Foam::volMesh]() * Grad_X’ On the other hand: gradU.T() & Grad_X seems to give the correct result. Thank you Last edited by N2a; August 19, 2009 at 12:47. 

August 19, 2009, 13:11 

#12 
Senior Member
Henrik Rusche
Join Date: Mar 2009
Location: Braunschweig, Niedersachsen, Germany
Posts: 277
Rep Power: 11 
Dear N2a,
Please, have a look into the Programmer's Guide (P24) and around. "*" represents the outer product. Hence, tensor * vector = third rank tensor which are not implemented. Probably you want the inner product, ie. vector & tensor = vector. Henrik 

August 21, 2009, 13:55 

#13 
Member
Sven Winkler
Join Date: May 2009
Posts: 70
Rep Power: 10 
Can someone explain what the line
Code:
const volVectorField & C=mesh.C(); How can I define a volVectorField with initial values, that is how can I define a volVectorField with defining a value of each of its components? Thank you! 

October 13, 2010, 02:55 

#14 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
Hello everybody,
I need to define a surfaceScalarField vector (1,0,0) which I have done as follows: volVectorField vectorv = vector(1,0,0); surfaceScalarField vectors = mesh.Sf() & fvc::interpolate(vectorv); But when I try to compile I have the following error in the first line: levelSetEqn.H:73: error: conversion from ‘Foam::vector’ to nonscalar type ‘Foam::volVectorField’ requested Does anybody know how can I define my surfaceScalarField? 

October 18, 2010, 07:39 

#15 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 14 
Your surfaceScalarField definition is fine. Your volVectorField definition is not. Check the constructors for a volField and use one of them to construct your volVectorField.


October 18, 2010, 09:21 

#16 
Senior Member
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 10 
Where can I check the constructors for a volVectorField?


October 18, 2010, 09:45 

#17 
Senior Member
Join Date: Mar 2009
Posts: 248
Rep Power: 11 
Dear Isabel
What you really need is to create a volumetric vector field i.e. a field in which: a vector is stored at the cell centre in the internalField; a vector is stored at the face centre on the boundaryField; What Eugene meant is that look for a previous declaration of some volVectorField and declare yours analogously. You are getting an error because you are trying to convert a vector to a field. This is not possible because the field needs information about the mesh so that it can calculate the size of the field. For your case your can do something like this : volVectorField vectorV ( IOobject ( "vectorV", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedVector("vectorV", dimless, vector(x,y,z)) ); Above given is just one option. This will create a volVectorField named vectorV. At each location a dimensionless vector with the components x,y,z is stored . Also the boundaryField type of this field is by default set to calculated. In case you want to have the same but a vector with dimensions then do the following: volVectorField vectorV ( IOobject ( "vectorV", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedVector ( "vectorV", dimensionSet( 0, 1, 1, 0, 0, 0, 0 ), vector(x,y,z) ) ); Now you have field with vector at each location which has dimesnions of velocity. Additionally if you want to presupply the boundaryField types then you can define: volVectorField vectorV ( IOobject ( "vectorV", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedVector ( "vectorV", dimensionSet( 0, 1, 1, 0, 0, 0, 0 ), vector(x,y,z) ), fixedValueFvPatchVectorField::typeName ); If you want to copy the boundaryField types of some already existing field then you can do something similar to what is done in the file interFoam/correctPhi.H. Have a look at that and you will understand how to do this . Hope that will help. Regards jaswi 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
CAE program for heat conducting  Rogerio Fernandes Brito  FLUENT  0  February 3, 2008 12:22 
Problem in program  tib  FLUENT  0  January 28, 2004 15:13 
How to write a simple program ??  kokey  FLUENT  0  March 19, 2002 11:21 
Benetton Formula 1  CD adapco Group Marketing  Siemens  13  February 7, 2002 10:33 
Any numerical triple integration program is available in Fortran?  Radhakrishnan  Main CFD Forum  3  March 4, 1999 02:03 