Laplacian(A*B)
 

Hello, is possible solve in openFoam a function laplacian(k,A*B) where k is constant, A is known volScalarField and B is searched unknown (volScalarField)?

Thanks
Richard

Did you consider fvm::laplacian(k*A,B)?

Yes I did, but I don't know if it is correct from mathematical point of view.
I need solve this:

dF/dt=laplacian(delta,P)
P is partial pressure and could be rewrite F = P / Psat
Psat is partial saturated pressure (function of Temperature)

I tried this, but without succes... :(
fvm::ddt(dw,F)=fvm::laplacian(delta*Psat,F)
fvm::ddt(dw,F)=fvc::laplacian(delta,Psat*F)

Thanks
Richard

when you say tried, but without success....what does that mean?

Could you not compile it?
Could you not run it?
Did it not yield the desired result?

fvm::ddt(dw,F)=fvm::laplacian(delta*Psat,F)

this should work and be your best bet...assuming Psat is just a constant.

just a note, but remember that
laplacian(k,AB) = div(k * grad(AB))
and is not, in general, equal to
laplacian(kA,B) = div(kA * grad(B))
only if A = const.

also
= is an assignement
== is checking if its equal

so in that implementation you should use ==

Not always: http://www.cfd-online.com/Forums/ope...-operator.html

true :)
sorry, should have clarified that I ment in this example

I have operator "==" in code, it is right, compile and solution done, but result is wrong, I think.

I write solver for Heat and Moisture transport in porous materials.
1 step - Temperature calculation (changing thermal parameters with moisture)
2 step - Humidity calculation (changing moisture parameters with temperature)
next Iterations...

Saturated Pressure is not a constant, it depends on temerature and the temperature is changing in time. Transport parameters are calculated in time and stored in volScalarFields.

Thanks
Richard

Hi Ricardo
how you have solved this equation?! with which solver of OF?

I started from basic Laplacian example, and still using PCG solver with DIC preconditioner, is it wrong?

No I just wanted to know.you are modifying the laplacianFoam,right? could you send me your case?

It is not problem, but it doesn't work correctly now, ...

I just like to know the way you are doing it.no problem.maybe an idea occurred to me.
my email is: force.of.love@gmail.com if you want to send it.

It has been send.

I am Ph.D. student, I would like use this program for simulations in my thesis. I wrote similar algorithm in 1D in Visual Basic, it works without any problem. OpenFOAM and C++ is new for me...
Richard

Dont forget the chain rule
 

Hi,

when psat is a function of temperature, you are not allowed to pull it out of the gradient in the laplacian function. But you could use the chain rule to get an implicit term of F and an explicit term of psat. Here we go:

Eqn (1): This is your starting point
Eqn (2): Split the gradient term
Eqn (3): Split the divergence term
Eqn (4): form the last two terms into laplacians again
Eqn 4 should work for you. Try it out.

Regards

Fabian

whats dw in these equations while it isn't in dF/dt?
how and why implicit terms convert to explicit ones and vice versa?

Hi

The first laplacian

accounts for the change in saturation pressure and would be zero for constant psat. It has to be treated explicit (fvc), as the conservation equation is for F. The second term

can be treated implicit (fvm) now due to the chain rule.

Regards

Fabian

Hi Niklas, laplacian(A)=d^2A/dx^2+d^2A/dy^2 in 2D but what means above laplacian(k,AB)?if they are multiply why laplacian(k,AB) is different from laplacian(kA,B)?

Thank you very much, I am going to try it. :)
Yesterday I used other approach (similar which I using in Visual Basic) for implicit scheme and I think that results was correct.

- generate fvscalarmatrix "mat" from laplacian(delta,F)
- multiply each cell in fvscalarmatrix mat by Psat in point of this cell (using lduAddressing)
- solve (fvm::ddt(dw,F)==mat)

But this code is more complicated and your approach seems better.

dw is aproximation function of sorption curve (relation between water content and relative humidity of air) it is nonlinear function, I forgot write in equation:o

Richard

The part "fvc::laplacian(delta*F,Psat)" causes stability problem,... :(

volScalarField F

internalField nonuniform List<scalar>
4000
(
0.503748
0.500001
0.5
0.5
0.5
0.5
0.49999
0.44179
-361.167
-2.31903e+06
0.500001
0.5
0.5
0.5
0.5
0.5
0.49999
0.44179
-361.165
-2.31902e+06

you could try to implement it implicitly
fvc::laplacian(delta*F,Psat) = fvc::div( delta*F*grad(Psat) )

volVectorField dps = delta * fvc::grad(Psat);
surfaceScalarField dpsf = fvc::interpolate(dps) & mesh.Sf();

then you can view the dps field as a 'convective' change of F due to the Psat gradient
and rewrite it like this

fvc::laplacian(delta*F,Psat) = fvm::div(dpsf, F)


...should work

Hi

That's a pitty. But the code of niklas seems to be promissing. Ricardo, I didn't get your approach in total. Could you explain it in a little more detail? Especially the part of the lduAddressing.

Regards

Fabian

implementation to solver >> solve (fvm::ddt(dw,F)==fvm::laplacian(lambdaD*Psat,F)+fv m::div(dpsf, F)); doen't works, too :(

This is my code, but it I am still working ...

a part of code ...
my approach to laplacian(labmbdaD,F*Psat) is in code, maybe for expert it could be ridiculous :D , but I am working with openFoam and C++ 2 weeks, and this code gives some "expected" values. Other approach gives unstability or doesn't work...

I tried next approach, rewrite partial pressure by gradient of temperature, it seems, that gives similar values like lduaddressing script :)

I don't know where is problem, I have to check all functions, material parameters and other properties again,...

thanks to all for support and advices
Richard

you REALLY need to be more specific when you say 'it doesnt work'.

I was wrong :o, It works, but obtained values ...

dimensions [0 0 0 0 0 0 0];

internalField nonuniform List<scalar>
4000
(
-1.35814e-10
4.58031e-11
4.58031e-11
4.58031e-11
4.5803e-11
4.58031e-11
4.58031e-11
4.58031e-11
-1.82592e-10
-1.77054e-12
-2.23032e-11

So it seems (two scheme unstable), that a problem could be somewhere else,

Is right using parameters (lambda), stored as volScalaField and (ununiform field) calculated in each step equation by this way? (fvm::laplacian(lambda,T)) Is it interpreted correctly to scheme or is used average values?

Thanks
Richard

Hi, anyone manage to solve the problem?

I face similar problem whereby I need to convert

to
I used eqn4 as recommended to get:
but seems like I can't place rho there in:
The error is "error: no matching function for call to ‘laplacian(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >, const rhoField&)’"

Another error is "note: template argument deduction/substitution failed"

Any idea how to solver it? Must been trying to solve it for a month.

Thanks