CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   How to add temperature to cavitatingFoam solver (http://www.cfd-online.com/Forums/openfoam/78767-how-add-temperature-cavitatingfoam-solver.html)

chodki-c August 2, 2010 03:28

How to add temperature to cavitatingFoam solver
 
Hi everyone,

I'm trying to solve a case which conjugates both multiphase flow and thermal wall. As I haven't found an appropriate solver I want to modify the cavitatingFoam solver. I just want to add an equation for temperature but I don't know how can I proceed.
The "HowTo add temperature to icoFoam" tutorial of Wiki cannot help me.

As anyone try to do the same thing and can help me!!

Have a good day :)

kathrin_kissling August 3, 2010 03:25

Hi,

can you explain, why this tutorial is'nt of any help?
Did you try the steps. In what step did you get problems?

Best Kathrin

chodki-c August 3, 2010 03:39

Hi Kathrin,

Thanks for your response.
The tutorial is made for the solver icoFoam.
I tought it was easy to do the same things with cavitatingFoam so I have followed all the steps without any changes.
However when I try to run the case "throttle" (which is the case example of cavitatingFoam) I meet some problems of dimensions:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.0-279cc8e8233b
Exec : thermalCavitatingFoam
Date : Aug 03 2010
Time : 09:35:57
Host : goth
PID : 4479
Case : /home/areelis/Bureau/Cynthia/tutorials/multiphase/thermalCavitatingFoam/throttle
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Reading thermodynamicProperties

Reading field p

Creating compressibilityModel

Selecting compressibility model linear
Reading field U

Reading field T

Reading/calculating face flux field phiv

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
expected a [ in dimensionSet
in stream ITstream : /home/areelis/Bureau/Cynthia/tutorials/multiphase/thermalCavitatingFoam/throttle/constant/transportProperties::DT, line 22, IOstream: Version 2.0, format ASCII, line 22, OPENED, GOOD

Selecting turbulence model type RASModel
Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
alphaK1 0.85034;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.85616;
gamma1 0.5532;
gamma2 0.4403;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
c1 10;
}

Courant Number mean: 0 max: 0
phiv Courant Number mean: 0 max: 0 acoustic max: 0.288861

Starting time loop

phiv Courant Number mean: 0 max: 0 acoustic max: 0.288861
deltaT = 1.1999e-08
Time = 1.1999e-08

DILUPBiCG: Solving for rho, Initial residual = 0.613556, Final residual = 0, No Iterations 1
max-min rho: 844.998 834.998
max-min gamma: 0 0
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 6.34307e-16, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 6.50228e-16, No Iterations 2
max(U) 2.83958
GAMG: Solving for p, Initial residual = 1, Final residual = 3.69146e-06, No Iterations 1
GAMG: Solving for p, Initial residual = 9.54005e-07, Final residual = 2.36346e-10, No Iterations 1
Predicted p max-min : 3e+07 1e+07
max-min gamma: 0 0
Phase-change corrected p max-min : 3e+07 1e+07
max(U) 2.80134
GAMG: Solving for p, Initial residual = 0.00996903, Final residual = 3.67993e-08, No Iterations 1
GAMG: Solving for p, Initial residual = 3.57757e-08, Final residual = 9.03801e-12, No Iterations 1
Predicted p max-min : 3e+07 1e+07
max-min gamma: 0 0
Phase-change corrected p max-min : 3e+07 1e+07
max(U) 2.79985
DILUPBiCG: Solving for omega, Initial residual = 5.23551e-05, Final residual = 1.62015e-12, No Iterations 1
DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 2.81372e-15, No Iterations 2
bounding k, min: 3.31924e-35 max: 9.99977 average: 9.99835


--> FOAM FATAL ERROR:
incompatible dimensions for operation
[T[0 0 -1 1 0 0 0] ] + [T[1 -3 -1 1 0 0 0] ]

From function checkMethod(const fvMatrix<Type>&, const fvMatrix<Type>&)
in file /opt/openfoam170/src/finiteVolume/lnInclude/fvMatrix.C at line 1194.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::error::abort() in "/opt/openfoam170/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 void Foam::checkMethod<double>(Foam::fvMatrix<double> const&, Foam::fvMatrix<double> const&, char const*) in "/opt/openfoam170/applications/bin/linuxGccDPOpt/thermalCavitatingFoam"
#3 Foam::tmp<Foam::fvMatrix<double> > Foam::operator+<double>(Foam::tmp<Foam::fvMatrix<d ouble> > const&, Foam::tmp<Foam::fvMatrix<double> > const&) in "/opt/openfoam170/applications/bin/linuxGccDPOpt/thermalCavitatingFoam"
#4
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/thermalCavitatingFoam"
#5 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#6
in "/opt/openfoam170/applications/bin/linuxGccDPOpt/thermalCavitatingFoam"
Abandon


So I think it's because the equation for the temperature is not the same for a multiphase flow.
Can you try to help me?
Thanks a lot in advance.

Bests. Cynthia.

kathrin_kissling August 3, 2010 03:47

Maybe it is something very simple

start with the first error output

expected a [ in dimensionSet
in stream ITstream : /home/areelis/Bureau/Cynthia/tutorials/multiphase/thermalCavitatingFoam/throttle/constant/transportProperties::DT, line 22, IOstream: Version 2.0, format ASCII, line 22, OPENED, GOOD

There seems to be something wrong in your transportProperties file. Some [ is missing. Could you start with checking that? Or post your transportProperties file. If this is correct we can take the next step if necessary!

Best
Kathrin

chodki-c August 3, 2010 04:21

Thanks,

I didn't see that mistake.
I have added the "[" but there is the same problem of dimension.

I have verified the dimensions of DT and T, but I think there is no problem here.
DT [ 0 2 -1 0 0 0 0]
T [0 0 0 1 0 0 0]

kathrin_kissling August 3, 2010 04:37

Ok,

could you post your implementation of the TEqn?

Maybe it is something there.

chodki-c August 3, 2010 04:48

4 Attachment(s)
Of course.
Please find enclosed the implementation of T and the case "throttle" with T.
Thanks a lot for your help again.

Cynthia

kathrin_kissling August 3, 2010 05:33

ok Cynthia,

in your TEqn:

Do

fvm::ddt(rho, T) +fvm::div(phi, T)

and in a first step skip the molecular transport. You need the rho, since you are not using the incompressible icoFoam, where the equations are devided by rho. Check with your dimension error and you will get the point.

This should work! I tried it myself just a minute ago.

Than you can start to add the next term.

If you have more questions feel free!

Best

Kathrin

chodki-c August 3, 2010 05:51

Thanks a lot!!!

It works well with your hints. I totally forgot that cavitatingFoam is a compressible solver and not icoFoam...

However when I introduce the laplacian term, I have the same problem of dimensions.
Can you explain to me this term. I'm quite new in OF and I'm not sure to understand it.

Bests.
Cynthia

jml September 30, 2010 11:21

hello everyone,
I have tried to add the temperature equation to cavitatingFoam as explained in the tutorial of wiki, but unfortunately I have the same problems of dimensions with the laplacian term.

-----------------
incompatible dimensions for operation
[T[1 -3 -1 1 0 0 0] ] + [T[0 0 -1 1 0 0 0] ]#0 Foam::error::printStack(Foam::Ostream&)
---------------------


Could you help me with the implementation? What can I do to solve it?

Thanks.


All times are GMT -4. The time now is 16:49.